XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Contact Analysis of Hip Joint in Ansys
 
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
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Mon Apr 14, 2014 2:43 am  Reply with quote

Dear all,

I have imported the femur and pelvis together with the articular cartilages of each on Ansys APDL as PARASOLID format.
Bones were meshed using Solid187 to model cortical bone and Shell181 to model trabecular bone. Cartilages were meshed using Solid187.

I have also modelled the muscles gluteus medius and gluteus minimus together with the ligament of the femur of the head using link elements; Link180.

In addition, I have used constraint equations (CE command) between the femur and its cartilage and the pelvis and its cartilage to prevent rigid body motion.
Boundary conditions were applied at the symmetrical boundary of the pelvis using a master node through the CERIG command.
A force and moment (which were calculated analytically) have been applied at the posterior end of the femur.

For the contact solution, the contact was set as the femoral cartilage (CONTA174) and target was set as the pelvic cartilage (TARGE170). Convergence was obtained; the femur experienced some rotation upwards, creating a penetration between the two cartilages.

My problem is this: I cannot plot any contact results such as; contact status, contact penetration, contact stress. When trying to plot any of these results, I obtain an error saying: "The requested CONT data is not available. The PLNSOL command is ignored."

I have tried to vary the normal stiffness coefficient, the friction coefficient, the penetration tolerance and the type of contact algorithm for the contact solution. But all yielded same results from the converged contact solution: small movement of femur and penetration of cartilages together with error message when trying to plot the contact results.

It would be helpful if someone could help me in rectifying this problem.

Thanks in advance.

Maria Kristina Agius
University of Malta
Back to top
View user's profile Send private message
jerome.drda
User


Joined: 21 Oct 2008
Posts: 10

PostPosted: Mon Apr 14, 2014 5:32 am  Reply with quote

Maria --

Here are a couple of quick suggestions, that, being quick, are not guaranteed: (1) Be sure to issue a "SET" command in the postprocessor to load the results from the results file into the active database. If that does solve the problem, then (2) it sounds as if the contact results have not been written to the results file. The "OUTRES" command provides control over this; you can issue "OUTRES,STAT" to see what its settings are. To get the contact results you're looking for, there should be something like "OUTRES,ESOL,ALL" or "OUTRES,MISC,ALL" before the SOLVE command.
Best of luck!
Jerry

Jerome F Drda
Lead Structural Analyst

Eaton
Aerospace Group
Fuel & Motion Control Systems Division
23555 Euclid Avenue
Cleveland, Ohio 44117-1795
tel: 216-692-6385
fax: 216-692-6639
JeromeFDrda@eaton.com
www.eaton.com/aerospace

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of maria.agius
Sent: Monday, April 14, 2014 5:43 AM
To: xansys@xansys.org
Subject: [Xansys] Contact Analysis of Hip Joint in Ansys

Dear all,

I have imported the femur and pelvis together with the articular cartilages of each on Ansys APDL as PARASOLID format.
Bones were meshed using Solid187 to model cortical bone and Shell181 to model trabecular bone. Cartilages were meshed using Solid187.

I have also modelled the muscles gluteus medius and gluteus minimus together with the ligament of the femur of the head using link elements; Link180.

In addition, I have used constraint equations (CE command) between the femur and its cartilage and the pelvis and its cartilage to prevent rigid body motion.
Boundary conditions were applied at the symmetrical boundary of the pelvis using a master node through the CERIG command.
A force and moment (which were calculated analytically) have been applied at the posterior end of the femur.

For the contact solution, the contact was set as the femoral cartilage (CONTA174) and target was set as the pelvic cartilage (TARGE170). Convergence was obtained; the femur experienced some rotation upwards, creating a penetration between the two cartilages.

My problem is this: I cannot plot any contact results such as; contact status, contact penetration, contact stress. When trying to plot any of these results, I obtain an error saying: "The requested CONT data is not available. The PLNSOL command is ignored."

I have tried to vary the normal stiffness coefficient, the friction coefficient, the penetration tolerance and the type of contact algorithm for the contact solution. But all yielded same results from the converged contact solution: small movement of femur and penetration of cartilages together with error message when trying to plot the contact results.

It would be helpful if someone could help me in rectifying this problem.

Thanks in advance.

Maria Kristina Agius
University of Malta






+-------------------------------------------------------------+
| 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)
_________________
Jerome F Drda
Structural and Fatigue Analyst

Eaton
Aerospace Group
Digital Prototyping Center of Excellence
23555 Euclid Avenue
Cleveland, OH 44117
Back to top
View user's profile Send private message
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Mon Apr 14, 2014 6:10 am  Reply with quote

Jerome,

Thanks for your prompt reply and help.

I have tried the SET command but obtained the same error when trying to plot the contact results.

I then issued the OUTRES,STAT command -- there were no settings listed --so this might be my problem. I have started running the solution after using the command OUTRES,ESOL,ALL -- will post here once I obtain a solution. Hope it works!

Thanks again,

Maria Kristina Agius
University of Malta
Back to top
View user's profile Send private message
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Mon Apr 14, 2014 3:13 pm  Reply with quote

Jerome,

I have run the solution using the OUTRES,ESOL,ALL command but am still not able to plot the contact results - I obtained the same error.

Please note that I have always been able to plot other results such as the Von Mises stresses however am having problems with the contact results, which are the ones I require.

Does anyone have any other ideas on how this problem may be fixed please?

Thank you.

Maria Kristina Agius
University of Malta
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: Mon Apr 14, 2014 3:34 pm  Reply with quote

Maria,

"outres, all" worked fine for me when I wanted to plot electrical contact resistance.

Also, I read on one of PADT's blogs that the undocumented command " rstsuppress,none" does the same. Didn't work for me but you could try it.


Best,
Ayo Brimmo
Masdar, UAE

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of maria.agius
Sent: 15 April 2014 02:14
To: xansys@xansys.org
Subject: Re: [Xansys] Contact Analysis of Hip Joint in Ansys

Jerome,

I have run the solution using the OUTRES,ESOL,ALL command but am still not able to plot the contact results - I obtained the same error.

Please note that I have always been able to plot other results such as the Von Mises stresses however am having problems with the contact results, which are the ones I require.

Does anyone have any other ideas on how this problem may be fixed please?

Thank you.

Maria Kristina Agius
University of Malta






+-------------------------------------------------------------+
| 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
danny.levine
User


Joined: 06 Jan 2009
Posts: 69

PostPosted: Tue Apr 15, 2014 5:21 am  Reply with quote

How much "penetration" is occurring at the acetabulum? Have you done a displacement plot to see the amount of motion? Try it with the displacement scaling set to 1.

This will help determine whether you might have missed contact altogether because the target and contact faces do not "see" one another. If you have used weak springs in your model, you can get a converged solution in which no contact occurs and yet the bodies don't appear to undergo rigid body motion.

DLL

Danny L. Levine, Ph.D., P.E.
Principal Engineer
Zimmer, Inc.

//www.zimmer.com
(574)372-4669 - Office
(574)298-4799 - Cell

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of maria.agius
Sent: Monday, April 14, 2014 5:43 AM
To: xansys@xansys.org
Subject: [Xansys] Contact Analysis of Hip Joint in Ansys

Dear all,

I have imported the femur and pelvis together with the articular cartilages of each on Ansys APDL as PARASOLID format.
Bones were meshed using Solid187 to model cortical bone and Shell181 to model trabecular bone. Cartilages were meshed using Solid187.

I have also modelled the muscles gluteus medius and gluteus minimus together with the ligament of the femur of the head using link elements; Link180.

In addition, I have used constraint equations (CE command) between the femur and its cartilage and the pelvis and its cartilage to prevent rigid body motion.
Boundary conditions were applied at the symmetrical boundary of the pelvis using a master node through the CERIG command.
A force and moment (which were calculated analytically) have been applied at the posterior end of the femur.

For the contact solution, the contact was set as the femoral cartilage (CONTA174) and target was set as the pelvic cartilage (TARGE170). Convergence was obtained; the femur experienced some rotation upwards, creating a penetration between the two cartilages.

My problem is this: I cannot plot any contact results such as; contact status, contact penetration, contact stress. When trying to plot any of these results, I obtain an error saying: "The requested CONT data is not available. The PLNSOL command is ignored."

I have tried to vary the normal stiffness coefficient, the friction coefficient, the penetration tolerance and the type of contact algorithm for the contact solution. But all yielded same results from the converged contact solution: small movement of femur and penetration of cartilages together with error message when trying to plot the contact results.

It would be helpful if someone could help me in rectifying this problem.

Thanks in advance.

Maria Kristina Agius
University of Malta






+-------------------------------------------------------------+
| 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 Send e-mail
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Tue Apr 15, 2014 11:57 am  Reply with quote

Dear Dr. Levine,

You are correct. My displacement reaches 9.77m at the far end of the femur, which was not evident from the automatically scaled plots I was analysing. Now that I have plotted the undeformed/deformed shape and the displacement using the true scale, it is clear that the femur has experienced rigid body motion even though convergence was obtained (please view images below).

I have run the solution at several different normal penalty stiffnesses; 0.1, 0.5,1,1.5,2,2.2,10 and also at 50 but the same results were obtained - same rigid body motion and displacement of the femur. Any ideas how I can prevent this from occurring?

I have also noticed that the femur becomes 2D and much larger in size, than the pelvis, once the true scale plots are plotted (view images below). Any ideas why?

PS. I have worked in SI units for this solution. Also, the distal end of the femur was chopped off to reduce the computation time during solution.

PPS. I have also attached an EPLOT of the assembly showing the boundary conditions and the loads on the full assembly (including the muscles and ligamentum teres). The force magnitude applied = 323.73 N and moment magnitude applied =26.484 Nm (these were calculated analytically)


Thanks for your help.

Maria Kristina Agius
University of Malta

Original BCs and Loads on Assembly:


Contact Solution Properties - Material ID set to Cartilage Material Model:


Deformed-Undeformed shape - Automatic Scale:


Deformed-Undeformed shape - True scale:


Displacement Vector Sum - True Scale - Zoomed Out


Displacement Vector Sum - True Scale - Zoomed In:


Von Mises Stress - Max at Ligament attachment to Pelvis. Shows Femur is now 2D:
Back to top
View user's profile Send private message
andrew.sims
User


Joined: 16 Jun 2009
Posts: 177

PostPosted: Tue Apr 15, 2014 8:28 pm  Reply with quote

Maria

Apologies if I have missed it. How have you engaged your contact? How many load steps and substeps are you using? As Danny mentioned you could have passed right through the contact pinball search region in a substep and missed it altogether.

Could be worthwhile using enforced displacements in a small initial load step to engage your contact and then remove that and ramp from the reactions to your desired force.

Have a look at the RKEY (ramping key) setting of DDELE.

Good luck

Andrew Sims
ResMed Ltd.
Back to top
View user's profile Send private message
danny.levine
User


Joined: 06 Jan 2009
Posts: 69

PostPosted: Wed Apr 16, 2014 5:11 am  Reply with quote

Since Andrew mentioned pinball radius, I suggest you check your value for that parameter. The pinball may be too small so that your contact and target nodes fail to detect each other.

I do agree with Andrew's comments about load step / substep size and the use of a small initial displacement step.

Other contact related suggestions to consider:
Use the Augmented Lagrange Formulation
Turn the nonlinear option "Line search" on


DLL

Danny L. Levine, Ph.D., P.E.
Principal Engineer
Zimmer, Inc.

//www.zimmer.com
(574)372-4669 - Office
(574)298-4799 - Cell

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of andrew.sims
Sent: Tuesday, April 15, 2014 11:28 PM
To: xansys@xansys.org
Subject: Re: [Xansys] Contact Analysis of Hip Joint in Ansys

Maria

Apologies if I have missed it. How have you engaged your contact? How many load steps and substeps are you using? As Danny mentioned you could have passed right through the contact pinball search region in a substep and missed it altogether.

Could be worthwhile using enforced displacements in a small initial load step to engage your contact and then remove that and ramp from the reactions to your desired force.

Have a look at the RKEY (ramping key) setting of DDELE.

Good luck

Andrew Sims
ResMed Ltd.






+-------------------------------------------------------------+
| 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 Send e-mail
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Wed Apr 16, 2014 5:16 am  Reply with quote

Thank you all for your help and replies. Am trying each of your suggestions one by one. Will post once I have results.

Regards,

Maria Kristina Agius
University of Malta
Back to top
View user's profile Send private message
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Sat Apr 19, 2014 1:58 am  Reply with quote

Dear all,

I have increased the pinball region factor (to a value of 10) and was obtaining convergence for the first few substeps, but then my solution stopped due to non-convergence.

I have also increase the number of sub steps, within the load step, using time step option in the solution controls (time at end=90, time step=3, min step=2, max step=6), but obtained same results as before.

Now am running the solution using line search option on, with an increase in pinball region factor (value of 5) and increased sub steps (as above).

Could the arc-length method option in Ansys help in my case?

Regarding using a small initial displacement step, and then reverting back to the load steps, I have understood the concept per se but have no idea how to implement it. Could someone kindly offer some help as to what commands/GUI settings must be set for a displacement driven solution?

Thanks once again,

Maria Kristina Agius
University of Malta
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Sat Apr 19, 2014 3:35 am  Reply with quote

On 19/04/2014 09:58, maria.agius wrote:
Quote:

I have increased the pinball region factor (to a value of 10) and was obtaining convergence for the first few substeps, but then my solution stopped due to non-convergence.

Good; getting a few sub steps to converge is definite progress. Getting
a difficult contact problem to fully converge can be challenging, as you
have found. When you got some converged solutions, what contact
formulation and contact stiffness were you using?


--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Sat Apr 19, 2014 8:34 am  Reply with quote

For the non-converged solution with pinball region factor set as 10, I used a contact stiffness of 1 and the Penalty method. The non-linear solution graph showed that the force was lowering and reaching the criterion, and then shifting back up in the next substep - it did this for quite a number of substeps until it shifted too high up and the solution stopped due to non-convergence.

Would the alteration of the contact stiffness obtain a converged solution with the same pinball region factor?

On another note; I have one force and one moment applied on my model - during the last solution the force was continuously shifting up and down and converging at each sub step (except the last one). However the moment was dropping down immediately and remaining at a much lower magnitude than the moment criterion. Could this be the problem?

Thanks

Maria Kristina Agius
University of Malta
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Sat Apr 19, 2014 9:19 am  Reply with quote

On 19/04/2014 16:34, maria.agius wrote:
Quote:
For the non-converged solution with pinball region factor set as 10, I used a contact stiffness of 1 and the Penalty method. The non-linear solution graph showed that the force was lowering and reaching the criterion, and then shifting back up in the next substep - it did this for quite a number of substeps until it shifted too high up and the solution stopped due to non-convergence.

Would the alteration of the contact stiffness obtain a converged solution with the same pinball region factor?

The general rule of thumb is that lowering contact stiffness will make
convergence easier but accuracy less good. Try reducing the contact
stiffness to 0.1. Are you using Augmented Lagrange formulation which I
think would be the best choice for your problem.

Quote:
On another note; I have one force and one moment applied on my model - during the last solution the force was continuously shifting up and down and converging at each sub step (except the last one). However the moment was dropping down immediately and remaining at a much lower magnitude than the moment criterion. Could this be the problem?

I don't think that is a problem.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
maria.agius
User


Joined: 14 Apr 2014
Posts: 9

PostPosted: Sun Apr 27, 2014 1:03 am  Reply with quote

Dear all,

I have managed to run a displacement driven solution on the model and obtain correct contact results :-)

Furthermore I have also run a solution using two load steps (using LS files), (i) the initial displacement solution (ii) the actual solution with loads at the distal end of the femur. Unfortunately, the solution is correct during the first load step, but then loses its position after the second load step, as seen by the MNTR file (attached image).

For the above solution, I used the command DDELE,4454,ALL, ,ON as suggested, to delete the applied displacement boundary condition and ramp up the loads from there in the second loadstep.

All of these were run with the same contact options; Contact stiffness was set to 0.1, Pinball region 5.

From the results, it seems that the second load step (load) is not being affected by the first load step (disp).

How should I proceed from the disp solution, which obtained correct results, to the actual load solution?

Thanks again,

Maria Kristina Agius
University of Malta


MNTR file:

[/code]
Back to top
View user's profile Send private message
jerzy.cwifeld
User


Joined: 02 May 2013
Posts: 39

PostPosted: Mon Apr 28, 2014 5:55 pm  Reply with quote

Did you run the two load step without leaving solution module? If you go to post processor after the firs load step you get two Load Step one.
Another solution to improve contact stability is to introduce spring elements that keep the parts together.
After you got converged solution you can run another load step with removed spring using EKIL.


Kindly regards
Jerzy Cwifeld
Structural Integrity Engineer/TM

OKG Aktiebolag
Box 220
101 24  Stockholm
Sweden
Klarabergsviadukten 90 entrance C (Visiting)

Phone +46491-78 65 17
SMS +4676-760 51 04
Fax +468-21 03 64
jerzy.cwifeld@okg.eon.se

www.okg.se
-----Ursprungligt meddelande-----
Från: Xansys [mailto:xansys-bounces@xansys.org] För maria.agius
Skickat: den 27 april 2014 10:04
Till: xansys@xansys.org
Ämne: Re: [Xansys] Contact Analysis of Hip Joint in Ansys

Dear all,

I have managed to run a displacement driven solution on the model and obtain correct contact results :-)

Furthermore I have also run a solution using two load steps (using LS files), (i) the initial displacement solution (ii) the actual solution with loads at the distal end of the femur. Unfortunately, the solution is correct during the first load step, but then loses its position after the second load step, as seen by the MNTR file (attached image).

For the above solution, I used the command DDELE,4454,ALL, ,ON as suggested, to delete the applied displacement boundary condition and ramp up the loads from there in the second loadstep.

All of these were run with the same contact options; Contact stiffness was set to 0.1, Pinball region 5.

From the results, it seems that the second load step (load) is not being affected by the first load step (disp).

How should I proceed from the disp solution, which obtained correct results, to the actual load solution?

Thanks again,

Maria Kristina Agius
University of Malta


MNTR file:

[Image: http://www.imageurlhost.com/images/um1boefim31v2qf5s9uo_thumb.png ] (http://www.imageurlhost.com/viewer.php?file=um1boefim31v2qf5s9uo.png)[/code]






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+
____________________________________________________________________________
Privileged/Confidential information may be contained in this message and is intended solely for the use of the addressee. If You receive this mail by mistake, You may not use, copy or distribute it to anyone else.<br/>Please erase the message and notify us immediately.
+-------------------------------------------------------------+
| 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
danny.levine
User


Joined: 06 Jan 2009
Posts: 69

PostPosted: Tue Apr 29, 2014 6:09 am  Reply with quote

Perhaps you don't want to remove ALL of the displacement constraints on your node 4454. Even if you were able to establish contact in load step 1, there may yet be rigid body motions possible. I would try keeping all constraints active except one that has the same orientation as your force. If that gives results that don't look right you might also remove M/L and A/P constraints.

Did you use a constraint equation or similar to connect node 4454 to a set of other nodes on the femur? If so, then I believe that node 4454 will have rotational degrees of freedom that need to be managed.

DLL

Danny L. Levine, Ph.D., P.E.
Principal Engineer
Zimmer, Inc.

//www.zimmer.com
(574)372-4669 - Office
(574)298-4799 - Cell

-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of maria.agius
Sent: Sunday, April 27, 2014 4:04 AM
To: xansys@xansys.org
Subject: Re: [Xansys] Contact Analysis of Hip Joint in Ansys

Dear all,

I have managed to run a displacement driven solution on the model and obtain correct contact results :-)

Furthermore I have also run a solution using two load steps (using LS files), (i) the initial displacement solution (ii) the actual solution with loads at the distal end of the femur. Unfortunately, the solution is correct during the first load step, but then loses its position after the second load step, as seen by the MNTR file (attached image).

For the above solution, I used the command DDELE,4454,ALL, ,ON as suggested, to delete the applied displacement boundary condition and ramp up the loads from there in the second loadstep.

All of these were run with the same contact options; Contact stiffness was set to 0.1, Pinball region 5.

From the results, it seems that the second load step (load) is not being affected by the first load step (disp).

How should I proceed from the disp solution, which obtained correct results, to the actual load solution?

Thanks again,

Maria Kristina Agius
University of Malta


MNTR file:

[Image: http://www.imageurlhost.com/images/um1boefim31v2qf5s9uo_thumb.png ] (http://www.imageurlhost.com/viewer.php?file=um1boefim31v2qf5s9uo.png)[/code]






+-------------------------------------------------------------+
| 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 Send e-mail
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