XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[Xansys] ANSYS Mechanical Restart Question
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
paul.troxler
User


Joined: 27 Aug 2013
Posts: 12

PostPosted: Wed Jun 03, 2015 9:58 am  Reply with quote

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
ayo.brimmo
User


Joined: 01 Jul 2013
Posts: 38
Location: Masdar City, Abu Dhabi

PostPosted: Wed Jun 03, 2015 10:48 am  Reply with quote

Check out the UPGEOM or UPCOORD commands. You can use them to add displacements from a result file/ previous analysis and update your geometry to the deformed geometry. The updated geometry can then be used for subsequent analyses.

On workbench (V15), if you activate the beta option from appearance settings, you can directly update a geometry with deformations from a .rst file by right clicking the geometry.

Best,
Ayo Brimmo
Research Engineer
Masdar, UAE

Quote:
On 3 Jun 2015, at 20:57, <ptroxler@borgwarner.com> <ptroxler@borgwarner.com> wrote:

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Ayo Brimmo
Research Engineer
Masdar Institute of Science and Technology
UAE.
Back to top
View user's profile Send private message
phil.erisman
User


Joined: 24 Jan 2012
Posts: 42

PostPosted: Wed Jun 03, 2015 1:39 pm  Reply with quote

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
janet.wolf
User


Joined: 25 Nov 2013
Posts: 27
Location: Houston, TX

PostPosted: Wed Jun 03, 2015 1:48 pm  Reply with quote

This is a topic we have been interested in, too. We've had some preload
scenarios that take more than a few hours, depending on available compute
resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS
product management about this, and they see the value in a solution to this
problem. Maybe more people can communicate this need to development and help
prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to
make restarts a viable option?

We have similar situations where the first load step is preloading up a
whole bunch of bolts before applying a number of different BC/loading
scenarios. So far our approach has been to simply live with the
computational overhead of solving the bolt preload step for each model
because we haven't found any other method that is better. Our models are
typically built so that the preload step converges reasonably well (perhaps
an hour or two tops of extra solve time on the cluster?) and this is
preferable to greatly complicating our workflow with restarts through RSM on
a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results
from one Mechanical static structural model as the initial conditions for a
second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and
contact pairs. The second model will have different contact settings with
temperature fields and external forces as the applied loads. We need to run
the first model once, then run the second model numerous times as we perturb
the applied loads & contact settings. The bolt-up step in model 1 is
computationally expensive. Hence the idea to use the output of model 1 as an
input for model 2.

The best idea we came up with is to export the first model's displacements
to a text file & import them into the second model. Then, using a command
snippet, create displacement arrays & use the "D" command to apply them as
BC's. It seems like the mechanics of these operations will work. However we
expect the results to be very wrong. First the bolt preload will not be
treated correctly (we need "locked" behavior in model #2's subsequent
steps). And the thermally induced stresses will be wrong because maintaining
the "D" command's setting will not allow the part to grow with the applied
temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
paul.troxler
User


Joined: 27 Aug 2013
Posts: 12

PostPosted: Thu Jun 04, 2015 4:34 am  Reply with quote

Greetins all,

Late yesterday I received an e-mail directly from tech support indicating their is an easier way. Details were not provided.

Regarding Ayo Brimmo's post:
We investigated combining UPCOORD & KUSE. It was not clear that it would give the correct result. Specifically, how is the bolt preload maintained as model #2 executes multiple subsequent steps. What puts the bolts in the "locked" mode? My co-worker was going to build a small test model. I haven't heard how that effort went.

Regarding Phil Erisman's post:
Given our model size & available resources, the initial bolt-up runs are on the order of 8-24 hours. (Some models are better behaved than others.) For now we are also repeating the boltup step for each model.

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com
828-650-7448
Back to top
View user's profile Send private message
danbohlen
User


Joined: 18 Aug 2008
Posts: 951
Location: Evendale OH

PostPosted: Thu Jun 04, 2015 5:58 am  Reply with quote

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis
STAR review chairman, Fan and Booster
GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines
Back to top
View user's profile Send private message
danbohlen
User


Joined: 18 Aug 2008
Posts: 951
Location: Evendale OH

PostPosted: Thu Jun 04, 2015 6:03 am  Reply with quote

I guess the part I might be missing from the original question:

Don't you preload the model (assembly) and then run operating conditions? So preload once, then maybe evaluating a bunch of operating conditions?

You would NOT want to reset preload just because the parts heat up or cool down or are put under load. You would expect that clamp load to vary in service - that's part of Ansys solution you are looking for.

Doing a bunch of studies with different assembly clamp up loads? Well use pre-tension elements (or other tricks listed in last email)


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis
STAR review chairman, Fan and Booster
GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 04, 2015 8:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines
Back to top
View user's profile Send private message
joseph.metrisin
User


Joined: 07 May 2009
Posts: 404

PostPosted: Thu Jun 04, 2015 6:11 am  Reply with quote

We use pretension a lot for bolted assemblies. First load case is pretension only, and to resolve the bolt preload, and all the other pilots/assembly fits can take a long time. This assembly step is the hardest one to get through and can eat 3/4 of the solution time or more before actual operating loads are applied. We usually assume zero friction since we consider it to be a worst case condition for pilots and clamped interface.

Back to the original question, I see no reason why you can't do a restart from the assembly condition. Read up on multiframe restart. It's not that hard.



Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office

(561)427-6191 Fax
JMetrisin@fttinc.com

Visit our website: www.fttinc.com

FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com

-----------------------------------------------------------------------------------------------------
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----------------------------------------------------------------------------------------------------


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 04, 2015 8:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH 45215
Build 90 Col K1.5 cube 1N152
M/D H110 1-513-243-2366




+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rod.scholl
User


Joined: 22 Oct 2010
Posts: 86

PostPosted: Thu Jun 04, 2015 6:27 am  Reply with quote

HI Dan -- I hear you about the ever-changing FKN value... with each release more intelligence is added to its internal calculation making it a moving target.

Here's a nice approach/tips (not using the PRET179's)

1. Use a *force* rather than a displacement. Then on load step 2, swap the force for the equivalent displacement (can be done without leaving /SOLU so no restart is necessary). This is basically what the PRET179 does. And then you can get it tensioned up in a single load step (though not necessarily single *substep* lol).

2. Also, consider a negative FKN value (is absolute stiffness, rather than a ratio) which won't change during the solve anymore -- this will let one at least iterate without chasing the changing FKN so it should only take 2 steps! More importantly, subsequent iterations after the clamped interface is established can soften/stiffen FKN (like if plasticity kicks in for example) and then the pretension-established distance get's invalidated (as does the bolt clamping analysis!).

3. Of course one can use KEYOPT 10 = 0 to stop some of the FKN movement

4. Finally, sometimes we can leverage the MPC algorithm instead of penalty/augemented lagrange, then all of this goes away because of zero-penetration. Of course that's for separation/bonded cases only, so it's not applicable in many bolt/flange analyses if you expect any prying/minor separation.

Bolted interfaces -- a never-ending source of the seemingly simple unveiling itself as complex!

BTW I concur that I just string the load cases together after the initial establishment of pretension -- unless we're doing high-yielding or proof or something. I figure we lost path-dependent accuracy early on with unknown friction at the interface, bolt-tightening sequence, etc. -- so I just stack 'em up in LS2, LS3, etc.! Or leverage single or multi-frame restarts (if in MAPDL).

Phew! -- met my quota today of nerdiness on FEA I think :).
______________________________
 
Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 4, 2015 7:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
keith.gallagher
User


Joined: 04 Aug 2014
Posts: 55
Location: Evendale, Ohio

PostPosted: Thu Jun 04, 2015 7:51 am  Reply with quote

Even if you hard code the FKN (Negative value), doesn't Augmented Lagrange change stiffness on the fly if the penetration tolerance is exceeded?
At least that's what I've often understood.

If in doubt I usually set the FKN using a negative value, use pure penalty method, and check the penetrations afterward to make sure it's ok.
Maybe that's overkill?

Keith Gallagher
GE Aviation



-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rod Scholl
Sent: Thursday, June 04, 2015 9:27 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

HI Dan -- I hear you about the ever-changing FKN value... with each release more intelligence is added to its internal calculation making it a moving target.

Here's a nice approach/tips (not using the PRET179's)

1. Use a *force* rather than a displacement. Then on load step 2, swap the force for the equivalent displacement (can be done without leaving /SOLU so no restart is necessary). This is basically what the PRET179 does. And then you can get it tensioned up in a single load step (though not necessarily single *substep* lol).

2. Also, consider a negative FKN value (is absolute stiffness, rather than a ratio) which won't change during the solve anymore -- this will let one at least iterate without chasing the changing FKN so it should only take 2 steps! More importantly, subsequent iterations after the clamped interface is established can soften/stiffen FKN (like if plasticity kicks in for example) and then the pretension-established distance get's invalidated (as does the bolt clamping analysis!).

3. Of course one can use KEYOPT 10 = 0 to stop some of the FKN movement

4. Finally, sometimes we can leverage the MPC algorithm instead of penalty/augemented lagrange, then all of this goes away because of zero-penetration. Of course that's for separation/bonded cases only, so it's not applicable in many bolt/flange analyses if you expect any prying/minor separation.

Bolted interfaces -- a never-ending source of the seemingly simple unveiling itself as complex!

BTW I concur that I just string the load cases together after the initial establishment of pretension -- unless we're doing high-yielding or proof or something. I figure we lost path-dependent accuracy early on with unknown friction at the interface, bolt-tightening sequence, etc. -- so I just stack 'em up in LS2, LS3, etc.! Or leverage single or multi-frame restarts (if in MAPDL).

Phew! -- met my quota today of nerdiness on FEA I think :).
______________________________
 
Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 4, 2015 7:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
joseph.metrisin
User


Joined: 07 May 2009
Posts: 404

PostPosted: Thu Jun 04, 2015 8:25 am  Reply with quote

Crap! I think we may have been doing our models wrong for a long time by ignoring the changing FKN issue. I wonder how much this affects bolt preload? I may make a request for a contact option that locks FKN at the end of a load step for more appropriate simulation of pretension clamped assemblies. I don't want to use the MPC contact option since we are interested in capturing flange openings.



Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office

(561)427-6191 Fax
JMetrisin@fttinc.com

Visit our website: www.fttinc.com

FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com

-----------------------------------------------------------------------------------------------------
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----------------------------------------------------------------------------------------------------


-----Original Message-----

HI Dan -- I hear you about the ever-changing FKN value... with each release more intelligence is added to its internal calculation making it a moving target.
_____________________________

Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
keith.gallagher
User


Joined: 04 Aug 2014
Posts: 55
Location: Evendale, Ohio

PostPosted: Thu Jun 04, 2015 8:38 am  Reply with quote

So if you stick with pure penalty and use a FKN factor does the resulting stiffness still change?

Or is this only a product of Augmented Lagrange?

Keith Gallagher
GE Aviation


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 04, 2015 9:03 AM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I guess the part I might be missing from the original question:

Don't you preload the model (assembly) and then run operating conditions? So preload once, then maybe evaluating a bunch of operating conditions?

You would NOT want to reset preload just because the parts heat up or cool down or are put under load. You would expect that clamp load to vary in service - that's part of Ansys solution you are looking for.

Doing a bunch of studies with different assembly clamp up loads? Well use pre-tension elements (or other tricks listed in last email)


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis
STAR review chairman, Fan and Booster
GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 04, 2015 8:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
mike.otto
User


Joined: 14 Jan 2012
Posts: 4

PostPosted: Thu Jun 04, 2015 8:49 am  Reply with quote

Allowing a floating FKN will definitely affect bolt tensions if temperature varies during subsequent load steps.
Keep keyopt,,10 set to 0 and enforce a constant contact stiffness when using the penalty method.

Learned this lesson the hard way...

Mike Otto
Tech Specialist II
Eaton Corporation
Vehicle Group Superchargers
19218 B Drive South
Marshall, MI  49068
269-781-0304 (wk)
269-377-1645 (cell)
http://www.eaton.com/


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rod.scholl
User


Joined: 22 Oct 2010
Posts: 86

PostPosted: Thu Jun 04, 2015 9:00 am  Reply with quote

Good stuff, Mike -- additionally, I think FKN get's changed when plasticity enters the model. I don't remember the rules, it might be *anywhere* in the model solve history and FKN get's cut by 10X... or maybe that's only if plasticity is present on the first load step, I don't remember... anyway, the rules change with each release, and my point is that Keyopt 10 =0 is an important safeguard, but not a fail-safe! Basically, relying on the FKN ratio means it's out of the operator's control. Now I should add, that in most cases the results aren't affected that much by the changing FKN... but if it ever did matter, bolted flanges would be a good candidate. Thus, going with negative FKN is the good way to go.

Of course non-changing FKN usually takes longer to converge... (ANSYS inc. is having the FKN change for a reason!)... so there's that too.

Here's an excerpt from our specialized course on contact/connections that has the important info of how to set negative FKN as Modulus*20/Length to mirror the typical start point for the FKN ratio=1:

<snip>
Ki = FKN * Modulus * 20 / L

. sometimes

It varies about this value - changes between releases.
There's an INT() function in there somewhere. Thin elements are also checked for (so L doesn't get too small).

It also gets lowered for plasticity...
... and large DOF problems -- presumably makes demo problems solve more quickly.
</snip>


______________________________
 
Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of MikeJOtto@eaton.com
Sent: Thursday, June 4, 2015 10:49 AM
To: xansys@xansys.org
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Allowing a floating FKN will definitely affect bolt tensions if temperature varies during subsequent load steps.
Keep keyopt,,10 set to 0 and enforce a constant contact stiffness when using the penalty method.

Learned this lesson the hard way...

Mike Otto
Tech Specialist II
Eaton Corporation
Vehicle Group Superchargers
19218 B Drive South
Marshall, MI  49068
269-781-0304 (wk)
269-377-1645 (cell)
http://www.eaton.com/


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
joseph.metrisin
User


Joined: 07 May 2009
Posts: 404

PostPosted: Thu Jun 04, 2015 9:01 am  Reply with quote

We do use keyopt(10)=0, but It seem that it could change in subsequent load steps which would muck up the preload. :(



Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office

(561)427-6191 Fax
JMetrisin@fttinc.com

Visit our website: www.fttinc.com

FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com

-----------------------------------------------------------------------------------------------------
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----------------------------------------------------------------------------------------------------


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of MikeJOtto@eaton.com
Sent: Thursday, June 04, 2015 11:49 AM
To: xansys@xansys.org
Subject: [FTT_SPAM] - Re: [Xansys] ANSYS Mechanical Restart Question

Allowing a floating FKN will definitely affect bolt tensions if temperature varies during subsequent load steps.
Keep keyopt,,10 set to 0 and enforce a constant contact stiffness when using the penalty method.

Learned this lesson the hard way...

Mike Otto
Tech Specialist II
Eaton Corporation
Vehicle Group Superchargers
19218 B Drive South
Marshall, MI 49068
269-781-0304 (wk)
269-377-1645 (cell)
http://www.eaton.com/


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
joseph.metrisin
User


Joined: 07 May 2009
Posts: 404

PostPosted: Thu Jun 04, 2015 9:05 am  Reply with quote

If I recall, ANSYS used to reduce FKN by 10x if any solid element attached to a contact pair went plastic. I think that behavior was changed around 2008-2009 so it didn't do that anymore.



Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office

(561)427-6191 Fax
JMetrisin@fttinc.com

Visit our website: www.fttinc.com

FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com

-----------------------------------------------------------------------------------------------------
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----------------------------------------------------------------------------------------------------


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rod Scholl
Sent: Thursday, June 04, 2015 12:01 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Good stuff, Mike -- additionally, I think FKN get's changed when plasticity enters the model. I don't remember the rules, it might be *anywhere* in the model solve history and FKN get's cut by 10X... or maybe that's only if plasticity is present on the first load step, I don't remember... anyway, the rules change with each release, and my point is that Keyopt 10 =0 is an important safeguard, but not a fail-safe! Basically, relying on the FKN ratio means it's out of the operator's control. Now I should add, that in most cases the results aren't affected that much by the changing FKN... but if it ever did matter, bolted flanges would be a good candidate. Thus, going with negative FKN is the good way to go.

Of course non-changing FKN usually takes longer to converge... (ANSYS inc. is having the FKN change for a reason!)... so there's that too.

Here's an excerpt from our specialized course on contact/connections that has the important info of how to set negative FKN as Modulus*20/Length to mirror the typical start point for the FKN ratio=1:

<snip>
Ki = FKN * Modulus * 20 / L

. sometimes

It varies about this value - changes between releases.
There's an INT() function in there somewhere. Thin elements are also checked for (so L doesn't get too small).

It also gets lowered for plasticity...
... and large DOF problems -- presumably makes demo problems solve more quickly.
</snip>


______________________________

Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of MikeJOtto@eaton.com
Sent: Thursday, June 4, 2015 10:49 AM
To: xansys@xansys.org
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Allowing a floating FKN will definitely affect bolt tensions if temperature varies during subsequent load steps.
Keep keyopt,,10 set to 0 and enforce a constant contact stiffness when using the penalty method.

Learned this lesson the hard way...

Mike Otto
Tech Specialist II
Eaton Corporation
Vehicle Group Superchargers
19218 B Drive South
Marshall, MI 49068
269-781-0304 (wk)
269-377-1645 (cell)
http://www.eaton.com/


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
keith.gallagher
User


Joined: 04 Aug 2014
Posts: 55
Location: Evendale, Ohio

PostPosted: Thu Jun 04, 2015 10:00 am  Reply with quote

At least this one I can say for sure. This is correct. It bit me hard when the change occurred.

Keith Gallagher
GE Aviation

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Metrisin, Joe
Sent: Thursday, June 04, 2015 12:05 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

If I recall, ANSYS used to reduce FKN by 10x if any solid element attached to a contact pair went plastic. I think that behavior was changed around 2008-2009 so it didn't do that anymore.



Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office

(561)427-6191 Fax
JMetrisin@fttinc.com

Visit our website: www.fttinc.com

FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com

-----------------------------------------------------------------------------------------------------
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----------------------------------------------------------------------------------------------------


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rod Scholl
Sent: Thursday, June 04, 2015 12:01 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Good stuff, Mike -- additionally, I think FKN get's changed when plasticity enters the model. I don't remember the rules, it might be *anywhere* in the model solve history and FKN get's cut by 10X... or maybe that's only if plasticity is present on the first load step, I don't remember... anyway, the rules change with each release, and my point is that Keyopt 10 =0 is an important safeguard, but not a fail-safe! Basically, relying on the FKN ratio means it's out of the operator's control. Now I should add, that in most cases the results aren't affected that much by the changing FKN... but if it ever did matter, bolted flanges would be a good candidate. Thus, going with negative FKN is the good way to go.

Of course non-changing FKN usually takes longer to converge... (ANSYS inc. is having the FKN change for a reason!)... so there's that too.

Here's an excerpt from our specialized course on contact/connections that has the important info of how to set negative FKN as Modulus*20/Length to mirror the typical start point for the FKN ratio=1:

<snip>
Ki = FKN * Modulus * 20 / L

. sometimes

It varies about this value - changes between releases.
There's an INT() function in there somewhere. Thin elements are also checked for (so L doesn't get too small).

It also gets lowered for plasticity...
... and large DOF problems -- presumably makes demo problems solve more quickly.
</snip>


______________________________

Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of MikeJOtto@eaton.com
Sent: Thursday, June 4, 2015 10:49 AM
To: xansys@xansys.org
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Allowing a floating FKN will definitely affect bolt tensions if temperature varies during subsequent load steps.
Keep keyopt,,10 set to 0 and enforce a constant contact stiffness when using the penalty method.

Learned this lesson the hard way...

Mike Otto
Tech Specialist II
Eaton Corporation
Vehicle Group Superchargers
19218 B Drive South
Marshall, MI 49068
269-781-0304 (wk)
269-377-1645 (cell)
http://www.eaton.com/


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
rod.scholl
User


Joined: 22 Oct 2010
Posts: 86

PostPosted: Thu Jun 04, 2015 10:20 am  Reply with quote

Thanks, guys -- I guess I can stop looking over my shoulder for this one!

The newer rule that reduces based on model size, presumably doesn't change from load step to load step -- so if there's no others working behind the curtain, maybe with Keyopt 10=0 one can be sure the FKN won't change mid-analysis after all and one can go with a FKN ratio? (though my paranoia might make me just enter a negative value just cuz).

Good conversation!

Rod

______________________________
 
Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Gallagher, Keith (GE Aviation, US)
Sent: Thursday, June 4, 2015 12:00 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

At least this one I can say for sure. This is correct. It bit me hard when the change occurred.

Keith Gallagher
GE Aviation

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Metrisin, Joe
Sent: Thursday, June 04, 2015 12:05 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

If I recall, ANSYS used to reduce FKN by 10x if any solid element attached to a contact pair went plastic. I think that behavior was changed around 2008-2009 so it didn't do that anymore.



Joseph T Metrisin
Structures Lead
Florida Turbine Technologies, Inc
1701 Military Tr. Suite 110
Jupiter, FL 33458 U.S.A.
+1 (561)427-6346 Office

(561)427-6191 Fax
JMetrisin@fttinc.com

Visit our website: www.fttinc.com

FTT's public email encryption keys are stored on the FTT Verified Directory at http://keys.fttinc.com

-----------------------------------------------------------------------------------------------------
Confidentiality Note:
The information contained in this transmission and any attachments are proprietary and may be privileged, intended only for the use of the individual or entity named above. If the reader of this message is not the intended recipient, you are hereby notified that any dissemination, distribution or copying of this communication is strictly prohibited. If you received this communication in error, please delete the message and immediately notify the sender via the contact information listed above.
-----------------------------------------------------------------------------------------------------


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Rod Scholl
Sent: Thursday, June 04, 2015 12:01 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Good stuff, Mike -- additionally, I think FKN get's changed when plasticity enters the model. I don't remember the rules, it might be *anywhere* in the model solve history and FKN get's cut by 10X... or maybe that's only if plasticity is present on the first load step, I don't remember... anyway, the rules change with each release, and my point is that Keyopt 10 =0 is an important safeguard, but not a fail-safe! Basically, relying on the FKN ratio means it's out of the operator's control. Now I should add, that in most cases the results aren't affected that much by the changing FKN... but if it ever did matter, bolted flanges would be a good candidate. Thus, going with negative FKN is the good way to go.

Of course non-changing FKN usually takes longer to converge... (ANSYS inc. is having the FKN change for a reason!)... so there's that too.

Here's an excerpt from our specialized course on contact/connections that has the important info of how to set negative FKN as Modulus*20/Length to mirror the typical start point for the FKN ratio=1:

<snip>
Ki = FKN * Modulus * 20 / L

. sometimes

It varies about this value - changes between releases.
There's an INT() function in there somewhere. Thin elements are also checked for (so L doesn't get too small).

It also gets lowered for plasticity...
... and large DOF problems -- presumably makes demo problems solve more quickly.
</snip>


______________________________

Rod Scholl
Principal | Epsilon FEA, LLC
Tel: 952.405.9710
Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of MikeJOtto@eaton.com
Sent: Thursday, June 4, 2015 10:49 AM
To: xansys@xansys.org
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Allowing a floating FKN will definitely affect bolt tensions if temperature varies during subsequent load steps.
Keep keyopt,,10 set to 0 and enforce a constant contact stiffness when using the penalty method.

Learned this lesson the hard way...

Mike Otto
Tech Specialist II
Eaton Corporation
Vehicle Group Superchargers
19218 B Drive South
Marshall, MI 49068
269-781-0304 (wk)
269-377-1645 (cell)
http://www.eaton.com/


+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
phil.erisman
User


Joined: 24 Jan 2012
Posts: 42

PostPosted: Thu Jun 04, 2015 1:19 pm  Reply with quote

I always have friction on from the start since I believe it helps prevent rigid body motion that might otherwise occur from parts squirting out from between frictionless contacts. What would be the rationale for having friction off for the first load step? Convergence issues?

Why do you use contact interference to model preload vs. the bolt pretension elements? Old habits? Or because PRET179 doesn't update for large deflection scenarios? I've always used the pretension elements and they seem like the easiest option to me but perhaps I'm missing something.

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 04, 2015 7:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
danbohlen
User


Joined: 18 Aug 2008
Posts: 951
Location: Evendale OH

PostPosted: Fri Jun 05, 2015 4:53 am  Reply with quote

Old habits, reusing existing models are the typical reasons.

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Thursday, June 04, 2015 4:19 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I always have friction on from the start since I believe it helps prevent rigid body motion that might otherwise occur from parts squirting out from between frictionless contacts. What would be the rationale for having friction off for the first load step? Convergence issues?

Why do you use contact interference to model preload vs. the bolt pretension elements? Old habits? Or because PRET179 doesn't update for large deflection scenarios? I've always used the pretension elements and they seem like the easiest option to me but perhaps I'm missing something.

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 04, 2015 7:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines
Back to top
View user's profile Send private message
danbohlen
User


Joined: 18 Aug 2008
Posts: 951
Location: Evendale OH

PostPosted: Fri Jun 05, 2015 5:00 am  Reply with quote

OK a couple of reasons we tend to turn friction off.

Physical: the parts, when assembled typically aren't put together in a fashion where the assembler is fighting friction. Not many press fit situations.

Numerical: We have seen odd results when friction is on. A rabbeted bolted joint that causes radial friction forces on nut and bolt face that really isn't there.

That being said there are a few occasions we'll do assembly runs of complicated assemblies where, in Ansys, we'd "assemble" parts A and B, turn friction on, and then continue with more parts.



-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Thursday, June 04, 2015 4:19 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I always have friction on from the start since I believe it helps prevent rigid body motion that might otherwise occur from parts squirting out from between frictionless contacts. What would be the rationale for having friction off for the first load step? Convergence issues?

Why do you use contact interference to model preload vs. the bolt pretension elements? Old habits? Or because PRET179 doesn't update for large deflection scenarios? I've always used the pretension elements and they seem like the easiest option to me but perhaps I'm missing something.

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Bohlen, Dan (GE Aviation, US)
Sent: Thursday, June 04, 2015 7:59 AM
To: ANSYS User Discussion List
Cc: Tomassetti, Vincent (GE Aviation, US); Myers, Henry (GE Aviation, US)
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

I might be missing the point of this thread, but here goes.....

Probably the biggest issue with preload I have is when I using surface to surface contact, no pretension elements, and I don't hard code in the contact element stiffness.

I get this - for example: I put a .005 interference and get say 10,000# of preload. If I need 20,000 you figure put .010 in right? Nope, cuz Ansys changes the contact stiffness (Which might be bigger issue we prolly need to specify the contact stiffness outright as Ansys might be changing the stiffness through the mission run as contact loads might go up and down).

We get the preload and continue from there with restarts.

The best way to do really difficult preload situations (multiple bolts, etc) is probably to use the pretension elements. Let Ansys interate internally.

Another trick I have employed when iterating on bolt clamp is to limit the # of equilibrium iterations and get an "unconverged" solution to see what clamp load I got. I figure the bolt clamp ought to be pretty well converged in 1-3 equil iterations. Adjust the nut/bolt head interference an only let the solution run all the way once I'm within tolerance.

Here's an aside question: when folks run assembly out there - do you have friction turned on from the onset or turn it on after bolt clamp and rabbet interferences are resolved (ie. Turn on friction with a restart.)?


Dan Bohlen
Senior/ SSt Engineer, Military HPT Analysis STAR review chairman, Fan and Booster GE Aircraft Engines
1 Neumann Way
Evendale, OH  45215
Build 90 Col K1.5   cube 1N152
M/D  H110  1-513-243-2366




-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Janet Wolf
Sent: Wednesday, June 03, 2015 4:49 PM
To: 'ANSYS User Discussion List'
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

This is a topic we have been interested in, too. We've had some preload scenarios that take more than a few hours, depending on available compute resources, so we've investigated restarts and UPGEOM. I've talked to ANSYS product management about this, and they see the value in a solution to this problem. Maybe more people can communicate this need to development and help prod things along?

Janet Wolf, PMP, PE
Trendsetter Vulcan Offshore
Janet.wolf@vulcanoffshore.com
Tel: 281-944-2824

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Erisman Philip
Sent: Wednesday, June 3, 2015 3:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question

Paul,

I'm curious as to why the bolt-up step is so computationally expensive as to make restarts a viable option?

We have similar situations where the first load step is preloading up a whole bunch of bolts before applying a number of different BC/loading scenarios. So far our approach has been to simply live with the computational overhead of solving the bolt preload step for each model because we haven't found any other method that is better. Our models are typically built so that the preload step converges reasonably well (perhaps an hour or two tops of extra solve time on the cluster?) and this is preferable to greatly complicating our workflow with restarts through RSM on a remote Linux cluster.

Would love to hear how others tackle this...

Phil Erisman
Engineering Analysis
John Deere

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of ptroxler@borgwarner.com
Sent: Wednesday, June 03, 2015 11:58 AM
To: xansys@xansys.org
Subject: [Xansys] ANSYS Mechanical Restart Question

Greetings all,

This morning a co-worker asked me how to perform a restart using the results from one Mechanical static structural model as the initial conditions for a second Mechanical static structural model.

The first model is a bolt-up analysis for an assembly - multiple bolts and contact pairs. The second model will have different contact settings with temperature fields and external forces as the applied loads. We need to run the first model once, then run the second model numerous times as we perturb the applied loads & contact settings. The bolt-up step in model 1 is computationally expensive. Hence the idea to use the output of model 1 as an input for model 2.

The best idea we came up with is to export the first model's displacements to a text file & import them into the second model. Then, using a command snippet, create displacement arrays & use the "D" command to apply them as BC's. It seems like the mechanics of these operations will work. However we expect the results to be very wrong. First the bolt preload will not be treated correctly (we need "locked" behavior in model #2's subsequent steps). And the thermally induced stresses will be wrong because maintaining the "D" command's setting will not allow the part to grow with the applied temperatures.

Does anyone have any suggestions/insight?

Regards,
Paul

Paul Troxler
Staff Engineer
BorgWarner, Inc.
1849 Brevard Road
Arden, NC 28704
ptroxler@borgwarner.com<mailto:ptroxler@borgwarner.com>
828-650-7448

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Dan Bohlen
Senior Staff Engineer
GE Aircraft Engines
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Fri Jun 05, 2015 11:59 am  Reply with quote

On Jun 5, 2015, at 7:00 AM, Bohlen, Dan (GE Aviation, US) wrote:

Quote:
Physical: the parts, when assembled typically aren't put together
in a fashion where the assembler is fighting friction.

Unless you're tightening threaded connections. Friction is the only
thing that keeps a threaded connection from spontaneously unscrewing
itself. Without friction you can't apply torque to a bolt. The only
way to assemble a bolt without fighting friction is to use a
tensioner of some sort.

As an aside, a primary purpose of structural bolting (and riveting,
to a degree) is to apply a clamping force between two surfaces to
prevent slip, which also tends to unscrew threads.

All the conversation about multiple ways of incorporating pretension
does have me wondering how to check your results against field
experience. After all the contact manipulations, you've got a highly
non-linear result, presumably path dependent. How do you know that
your connection ships with the same pretension as you figured? How do
you even know that the pretension you incorporate is the value that
will actually serve the purpose? Shouldn't the fastener size and pre-
load be the result of the analysis, rather than the input?

Just sayin'…after all it's Friday.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
phil.erisman
User


Joined: 24 Jan 2012
Posts: 42

PostPosted: Fri Jun 05, 2015 1:41 pm  Reply with quote

"How do you know that your connection ships with the same pretension as you figured?"

We don't of course... Analytical pretension input values are based on torque specs given to manufacturing and some reasonable assumptions regarding k-factor. The k-factor varies of course as does how much torque is actually applied on the assembly line. We know our analytically applied pretension value does not necessarily match the reality of a given bolt coming off the assembly line and have some conservatism baked into the process.

"How do you even know that the pretension you incorporate is the value that will actually serve the purpose?"

In our analysis department this is the question we try to answer. Designs are created based on past history, hopefully some hand calcs, and manufacturing concerns and considerations. Analysis results will then drive changes to bolt patterns, sizes, etc. in order to satisfy our requirements for a given product's intended function.

Phil Erisman
Engineering Analysis
John Deere


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Christopher Wright
Sent: Friday, June 05, 2015 1:59 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] ANSYS Mechanical Restart Question


On Jun 5, 2015, at 7:00 AM, Bohlen, Dan (GE Aviation, US) wrote:

Quote:
Physical: the parts, when assembled typically aren't put together in a
fashion where the assembler is fighting friction.

Unless you're tightening threaded connections. Friction is the only thing that keeps a threaded connection from spontaneously unscrewing itself. Without friction you can't apply torque to a bolt. The only way to assemble a bolt without fighting friction is to use a tensioner of some sort.

As an aside, a primary purpose of structural bolting (and riveting, to a degree) is to apply a clamping force between two surfaces to prevent slip, which also tends to unscrew threads.

All the conversation about multiple ways of incorporating pretension does have me wondering how to check your results against field experience. After all the contact manipulations, you've got a highly non-linear result, presumably path dependent. How do you know that your connection ships with the same pretension as you figured? How do you even know that the pretension you incorporate is the value that will actually serve the purpose? Shouldn't the fastener size and pre- load be the result of the analysis, rather than the input?

Just sayin'...after all it's Friday.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+
+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Fri Jun 05, 2015 2:21 pm  Reply with quote

On Jun 5, 2015, at 3:40 PM, Erisman Philip wrote:

Quote:
We don't of course...

Quote:
"How do you even know that the pretension you incorporate is the
value that will actually serve the purpose?"

In our analysis department this is the question we try to answer.

Those were rhetorical questions. I knew the answers already or
thought I did, based on about 50 years of exposure to bolted
connections. I was curious about whether anyone's field experience
might be better than my own.

There are some more-or-less ball park accurate ways to preload a
bolt. A torque wrench is the least accurate with 30-40% error because
of the unpredictability of friction. Turn-of-the-nut with a very
carefully assembled bolt is about the best way, short of a
tensiometer, but it's only accurate within 10% or so). But my own
feeling is that safety wire (or a cotter pin) is the only 100%
reliable way to make sure a bolt stays put.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum
You cannot attach files in this forum
You cannot download files in this forum


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron