Home.Forum.Subscribe.Account.Rules.Resources.FAQ.ANSYS Links.
Home > FAQ

Other Resources

1. Where are there other ANSYS FAQ's
2. What are some other ANSYS Resources on the Web?

XANSYS List Questions

3. What is XANSYS?
4. How did XANSYS Start?
5. What is XANSYS Not?
6. Who runs XANSYS?
7. What the heck dow RTFM stand for?
8. Why was my membership rejected?
9. Why was unsubscribed?
10. Why didn't anyone answer my question?
11. Why is there a forum and a list server?

ANSYS Installation

12. I am struggling to get ANSYS to install. I am having licensing problems. What should I do?
13. I am ready to switch over to Linux. What version of the OS do I need?
14. Why do I get a license error after I just installed a new version of ANSYS or service pack?

Geometry Import

15. Why do I get errors when I try and import an IGES file?
16. What is the best format for Geometry Import into ANSYS?
17. What can I do to improve my success with Geometry Import?
18. What is a *.anf file? How do I get the format of the *.anf File? Why is there an *.anf file in my directory after I import something.

Modeling in ANSYS

19. What is Design Modeler?
20. What is the geometry engine in ANSYS?
21. What can I do about Boolean operation failures?
22. How do I find out the number for the kp/line/area/volume I just created?

Meshing

23. ANSYS, Inc. has so many meshers, which one should I use?
24. Can I use Tetrehedral elements?
25. What is the best way to create a Hex (brick) mesh?
26. My mesh keeps failing, how can I find out where it is having problems?
27. Little slivers are giving me fits, what can I do?
28. How good is my mesh?
29. How do I connect Tet and Hex elements?
30. My model is too dang big, what can I do?

Structural Analysis

31. Waiting for Questions...

Dynamic Analysis

32. Waiting for Questions...

Post Processing

33. Waiting for Questions

APDL

34. Waiting for Questions

Contact

35. Contact Background
36. On what factor can a contact analysis be judged as "OKAY"?
37. What affects the accuracy and convergence of a contact analysis?
38. What is Hertz Stiffness? How is it calculated?
39. Simulating contacts between 2 Rubber material bodies. How can I evaluate E for the rubber so that I can roughly estimate the contact Stiffness?
40. While using NTN contact elements between two (3D) surfaces, is there any recommended practice for meshing at those two surfaces?
41. What are the guidelines to estimate FKN for a contact Analysis.
42. When two different material (say Steel and Aluminum) are in Contact, which material's E should be considered for evaluating FKN
43. How to specify Sticking and Sliding conditions for Contact between two bodies?
44. How to estimate TAUMAX?
45. I have Higher order elements (with mid-side nodes) on the two contacting surfaces & I want to analyse the problem using NTN Contact. Can I create NTN Contact between the mid-side Nodes?
46. While editing the real constants of a Contact element, like FKN can negative values be entered?
47. How does FTOLN affect convergence & Accuracy of results?
48. How and where is contact detected?
49. There are several Contact Surface behaviour options on the Contact Wizard. What does each one of them do/describe?
50. How should I simulate interference? Between two parts there exists both interference as well as Gap between their surfaces? Using STS Contact element, what factors need to be adjusted/set ?
51. RIGID body motion error. I have the FE model with well defined constraints. Yet I see this error in the very beginning of the Solution. How can I avoid this error?
52. In a Flexible-Flexible body contact, Why should the surface with finer Mesh be designated as Contact Surface, and the other surface (with coarse mesh) be designated as Target?
53. Guidelines to choose Target/Contact Surface
54. What is Pinball Region ? What does it affect? What is its purpose in Contact Analysis?
55. What type of Contact is best suited to simulate Interference fit kind of problems? NTN type of Contact is best suited to simulate Interference Fit kind of problems. Most interference problems have negligible relative sliding deformation.
56. For NTN elements, how should the axis of NTN element be oriented? (I-J orientation of element)

Other Resources

1. Where are there other ANSYS FAQ's

There are a couple of FAQ's on the web:

Return to Top

2. What are some other ANSYS Resources on the Web?

The best place to go for ANSYS related information is www.ansys.net. A site dedicated to all things ANSYS hosted and run by Sheldon Imaoka. From here you can find links to the rest of the ANSYS world as well as much of the information summarized in this FAQ. You may also want to do a search of PADT's "the Focus" newsletter for articles on the topic you are interested in.

Return to Top

XANSYS List Questions

3. What is XANSYS?

XANSYS is "a place for the ANSYS user community to exchange ideas and help each other be more productive." 

It is a list for professional users and students who are doing serious work with ANSYS software.  It is a bit formal and strict so that it can stay focused on sharing ANSYS expertise across the sales community.

The community interacts through one of two systems that have idenitcal content:  an Online Forum and a Mail List Server.

The XANSYS mail server is an "old school" mail list server that sends a copy of any messages sent to the list to all members of the list.  It also sends a copy to the forum so that the content in both places is identical.  It uses mailman as its server

The XANSYS Forum is a new interface that is more "web 2.0"  and is a very typical user forum that allows anyone to view the content, and allows members to post new topics and reply to existing ones.  When a post is made, a copy is sent to the mail server so those who interact through e-mail, will get a copy.  It uses phpBB as its server.

 

Return to Top

4. How did XANSYS Start?

The lore is that Dan Bohlen of GE Aircraft Engines started the list in a previous geological epoch.

Learn more on the History Page.

Return to Top

5. What is XANSYS Not?

XANSYS is not a place to:

  • Get free technical support
  • Argue or pick fights
  • Bitch about ANSYS or ANSYS related issues
  • Look for help on homework
  • Discuss politics, religion or your personal obsessions

Return to Top

6. Who runs XANSYS?

XANSYS is administered and monitored by Martin Liddle  and Fern Thommasy.  They do 95% of the work associated with the list. The software and hardware are provided by PADT.  Jason Krantz from PADT does the sysadmin work.

Return to Top

7. What the heck dow RTFM stand for?

Often times new users will pose a question that can be answered if they spent a little bit of time reading the manual. In fact, the ANSYS manuals are actually very good once you understand how they are organized. Many experienced users gained most of their knowledge by reading the manual. So, when they see a question that is pretty obviously in the manual, they say: "Read the F&^%*$# Manual!" 

Many lists and forums ban RTFM as a response, this list does not.  For more on RTFM see: http://en.wikipedia.org/wiki/Rtfm

Return to Top

8. Why was my membership rejected?

Most of the time a membership request was rejected because the requestor did not follow the instructions on how to sign up. Please read the instructions and try again.

Another reason for rejection is that you gave an e-mail address from a free server such as Yahoo or Hotmail. XANSYS does not except membership from large, free e-mail sites since past experience has shown that posters from such sites are either spammers or feel that the anonymity of a generic domain name allows them to behave inappropriately.

A third reason is that you are from a country that is not authorized to use ANSYS.

Return to Top

9. Why was unsubscribed?

You were probably unsubscribed for one of two reasons: You violated a rule on the list or your mail server rejected too many messages. Check your inbox for an unsubscribe notification.

Return to Top

10. Why didn't anyone answer my question?

There are three general reasons why questions go unanswered:

  1. The question was poorly asked. Try again with more specifics and explain why you want to do it as well.
  2. You did not include your full name and company/university in your posting. Members do not respond unless you include this information.
  3. No one knows the answer.

Return to Top

11. Why is there a forum and a list server?

XANSYS started as a list server and has been very successful over the years, even more successful than many on-line forums.  We feel that the list server approach is superior for this type of list because the participants tend to be very busy engineering professionals and they just don't have time to go browsing through a forum every day.  That requires a proactive involvement in the community.  A list server is reactive in that you automatically receive e-mails and you can glance at them in passing to see if one interests you or you want to respond to one.  On forums, you tend to get one or two people who spend all day watching the forum answering most of the questions. 

But, forums have a huge advantage in terms of organization information and following topic threads.  And many younger users only know how to interact in an online community through forums.  So XANSYS decided to do both.  Leave the reactive list server there but also allow people who were proactive and who felt more comfortable on forums, interact that way.

Having a Forum also provides the added advantage of getting a searchable archive "for free."

As with everything on XANSYS, if you don't like it, you can start your own list or forum.

 

Return to Top

ANSYS Installation

12. I am struggling to get ANSYS to install. I am having licensing problems. What should I do?

Call your official ANSYS support provider. These types of issues are best resolved by the tech support provider that you are paying for. If you are not paying for technical support, please don't go asking for help on XANSYS.

Return to Top

13. I am ready to switch over to Linux. What version of the OS do I need?

See your instillation manual for the official supported version. This is what ANSYS, Inc. will support. Other versions work and you should search the XANSYS archives for any threads on the subject. If you can't find any, post a request for other people's suggestions but make sure you include your hardware specification and the OS versions you want to use.

Return to Top

14. Why do I get a license error after I just installed a new version of ANSYS or service pack?

There are two common causes of this problem.

First, the latest version of your license file needs to be loaded on the server. The TECS end date in the file needs to be later than the creation date of the ANSYS version you're trying to run. Usually the license files are emailed to the ANSYS Support Coordinator at your organization when your TECS is renewed.

Second, the correct version of the ANSYS license manager needs to be loaded on the server. Check the installation manual for the proper version numbers.

Return to Top

Geometry Import

15. Why do I get errors when I try and import an IGES file?

Errors during import are usually caused by an error in the IGES file or by tolerance problems. The easiest way to check for a bad file is to try and read the file in to a CAD package and see if it has problems. If it doesn't work then you need to go back to the source and try and clean up the geometry there.

You also need to be careful about how you get the file to your computer. IGES files are text (ASCII) files and they can get mangled by FTP or e-mail programs. Your best bet, for speed as well as robustness, is to zip the file before you transfer it. Zip'ing will compress the file and convert it into a more robust binary. If you don't zip and you use FTP, make sure you are in ASCII mode for the transfer.

Tolerance problems are trickier to solve. They are caused by the fact that the CAD system that created the geometry defines "close" differently then ANSYS. In fact, ANSYS defines "close" as very close and is considered a "tight" geometry representation. The most common error message for this is "Line does not lay on area" and sometimes a message about twisted surfaces. See suggestions below on how to avoid these.

Return to Top

16. What is the best format for Geometry Import into ANSYS?

The best format depends on your CAD system and the geometry you work with. In general, the direct translators from a specific CAD system work much better then IGES. Parasolids files work well too.

Return to Top

17. What can I do to improve my success with Geometry Import?

There are a couple of things you can do to make Geometry Import more robust:

  • Use the direct CAD translator if available
  • Use Parasolid files. The Parasolids translator in ANSYS has "healing" routine that can fix a lot of problems.
  • Set your tolerances in your CAD system tighter
  • Defeater you model. Many problems are caused by small features that you are going to mesh over anyhow.
  • Use a CAD cleanup tool like CadFix. PADT has had a lot of success with this.
  • Use design modeler to create your geometry or at least import it and save as *.anf.

Return to Top

18. What is a *.anf file? How do I get the format of the *.anf File? Why is there an *.anf file in my directory after I import something.

ANSYS can read and write its own geometry file called an ANSYS Neutral File and it has the file extension of .anf. It is a formatted file so you will need a copy of the manual "Guide to Interfacing with ANSYS" to understand what is in there.

The file is also created when you import geometry with a direct translator and is left in your directory.

Return to Top

Modeling in ANSYS

19. What is Design Modeler?

Design Modeler is the geometry import/modify/creation tool for the new Workbench interface. It is significantly more robust then the ANSYS modeler. For more info, see PADT's DM FAQ

Return to Top

20. What is the geometry engine in ANSYS?

The insides of the geometry engine in ANSYS have evolved to be a bit complex. Someone from ANSYS, Inc. development may know the details but the rumor is that there are two geometry kernels: a home grown NURBS kernel and a purchased kernel called XOX. Both are NURBS based b-rep solid modeling kernels.  XOX the company no longer exists.

Return to Top

21. What can I do about Boolean operation failures?

The first trick to Boolean operations is to understand the BTOL command. The value of BTOL is the "point coincidence" value for Boolean operations. What this means is that when you add, glue or subtract areas or a line, the geometry engine considers any two points to be identical if they are within the BTOL value. If you have sloppy geometry you may want to increase this value. If you have a lot of Boolean operations you may want to start with it smaller to create tighter geometry. The use of BTOL is a bit of an art and the best way to get a feel for it is to try it out on your models.

  • Some other tricks are:
  • Keep your operations to a minimum
  • Try not to do operations on geometry that very slightly overlaps
  • Don't do operations that result in very small pieces of geometry (slivers). Even if the work, future commands may not.
  • Consider building your geometry from the bottom up rather then using Boolean operations
  • Consider using DesignModeler or your CAD package

Return to Top

22. How do I find out the number for the kp/line/area/volume I just created?

When you execute a command in ANSYS that creates a single entity, the number of the new entity is often stored in a hidden APDL variable called _return. This is not always documented so you need to try it and see if it works for what you are trying to do.

If you are creating multiple entities or _return isn't filled, then there are two common solutions. The first is to set the NUMSTR,type,value to some number that you know that is larger then your current highest number. Any new entities will start numbering at this value and increase by 1 for each additional entity.

The second solution is to use components creatively. Create a component of the selected entities before the operation then unselect that component to grab all the new entities. You can then use *get's to determine entity numbers or just throw them into a new component.

Return to Top

Meshing

23. ANSYS, Inc. has so many meshers, which one should I use?

That depends on what you want to do. There are so many meshers because there are so many different needs out there. In general, the meshers in ANSYS produce a very high quality mesh that tends to have less elements then other meshers. It does take more direction from the user to get that mesh though. The user control available also allows the user to get the exact mesh they are looking for. There are several meshers for each element shape. If you are unhappy with the default tet, tri or quad meshers, then take a look at the MOPT command in the manual for information on changing the default algorithms.

The workbench mesher is very similar but automates a lot of steps such that it is much more robust, but the quality of the mesh not be as good as can be obtained with all of the controls in ANSYS (this will change over time).

The ICEM CFD meshers are fantastic for CFD and field type problems, especially if you have a large problem. The brick mesher in the ICEM CFD products is fantastic (see below). If you do large sheet metal assemblies, the surface mesher in ICEM CFD is also quite good.

Experience has shown that knowing your meshing tool inside and out is more important then which tool you use. Take time to get to know all the options and play around some.

Return to Top

24. Can I use Tetrehedral elements?

If you are solving using one of the ANSYS solvers then a Tet mesh, with midside nodes, should work, and may even create more accurate results then a distorted Hex mesh. If you are working with thin structures, then you should consider shell elements of some type rather then thin Tets or Hexes. Bricks (hex's) are more efficient but if they become distorted or you compromise geometry to create a mesh, the Tet's are preferred. The exception to this is when solving with Ls-DYNA. It is much more accurate with Hex's then with Tet's.

Return to Top

25. What is the best way to create a Hex (brick) mesh?

Again, that depends on your geometry. The HEXA mesher in ICEM CFD and AI*Environment is by far the most capable and powerful hex mesher available. It will work on almost any situation and allows the user to store mesh layouts for use on similar geometry, saving a huge amount of time. If you don't have access to HEXA, then the secret to Hex meshing is to extrude your mesh. Both ANSYS and Workbench have nice capabilities in this area. The key is slicing up your geometry into sweepable volumes. See the manual for more on this.

Return to Top

26. My mesh keeps failing, how can I find out where it is having problems?

When meshing in ANSYS, if you get a failure on an area or volume the error message sometimes give you feedback on what happened. If it doesn't give enough, then look at the area or volume that failed, often the problem is obvious that you need more elements. If you need further information, then turn element shape checking off before you mesh, shpp,off. Then mesh the offending entities. After the mesh is created turn shape checking back on with shpp,on. Then use CHECK,ESEL to select elements with errors. Use GPLOT to plot lines and elements to see the bad elements and where they are located.

Return to Top

27. Little slivers are giving me fits, what can I do?

The first solution is to try and get rid of them where they were created. If you can't do that a good solution is to pre-mesh all the slivers one at a time before you do a vmesh or an amesh,all. If that doesn't work then you should try Workbench or ICEM CFD. They can mesh over slivers and they both allow you to merge areas to eliminate slivers.

Return to Top

28. How good is my mesh?

There are diagnostic tools in ANSYS and in Workbench (FEModeler). Any mesh should show a minimal amount of warning elements using these tools. However, mesh quality is much more then that. Some pointer are:

  • Make sure you have no abrupt changes in element size
  • Make sure you have enough refinement to capture local geometry changes
  • Look at your unaveraged results. There shouldn't be significant change between touching elements and the unaveraged and averaged values should be close.
  • If you are conserned, keep refining the mesh until your result values stop changing.

Return to Top

29. How do I connect Tet and Hex elements?

TBA

Return to Top

30. My model is too dang big, what can I do?

TBA

Return to Top

Structural Analysis

31. Waiting for Questions...

TBA

Return to Top

Dynamic Analysis

32. Waiting for Questions...

TBA

Return to Top

Post Processing

33. Waiting for Questions

TBA

Return to Top

APDL

34. Waiting for Questions

TBA

Return to Top

Contact

35. Contact Background

Primarily contributed by M Shashikanth back in 2003.

Terminology:

  • STS - Surface to Surface Contact
  • NTS - Nodes to Surface Contact
  • NTN - Node to Node Contact
  • FKN or Kn - Normal Contact Stiffness
  • E - Youngs Modulus ICONT - Initial Contact value
  • PMIN & PMAX - Minimum and Maximum initial Penetration range
  • PINB - Pinball region Radius
  • FTOLN - Penetration tolerance Mu - Friction Coefficient

Return to Top

36. On what factor can a contact analysis be judged as "OKAY"?

Penetration. In physical reality, penetration between 2 contacting bodies never occurs. This is a mathematical creation so as to activate a contact stiffness between two bodies. Keeping penetration to a minimum is a best way to simulate a contact analysis. For achieving this, the contact Stiffness may be specified as high as possible as long as a converged FE solution is possible.

Return to Top

37. What affects the accuracy and convergence of a contact analysis?

(FKN) Stiffness used for the Contact is a major factor affecting Convergence of Contact problems. Using Higher values of Stiffness may diverge the solution. Its advised to start with a small enough value and get a converged solution. Re-solve with increased value of stiffness so long as the problem stops converging. Trial-and-Error + Experience will help you predict the Contact Stiffness needed to solve a Contact Analysis. Another recommended practise is to run the analysis with an initial small contact stiffness and then slowly increase the stiffness over a series of load steps. This will ramp the contact stiffness value from the initially considered Stiffness, thus improving convergence behavior. The results for the last loadstep would have been analyzed with more stiffness and hence would be more accurate than previous results.

Return to Top

38. What is Hertz Stiffness? How is it calculated?

Hertz Stiffness provides an approximate value for the Penalty Stiffness value. Kh = l*E where, Kh --> Hertz Stiffness l --> Size/edge length of the element at the contact surface E --> Youngs Mod of Contact Surface For 2D models, the thickness of element is considered for l

Return to Top

39. Simulating contacts between 2 Rubber material bodies. How can I evaluate E for the rubber so that I can roughly estimate the contact Stiffness?

Consider E for the rubber material portion as: E = 6(a+b) where a and b are the first two Mooney-Rivlin contants

Return to Top

40. While using NTN contact elements between two (3D) surfaces, is there any recommended practice for meshing at those two surfaces?

Meshing between the two sides were varying along X. Surface 1

- - - - - - - - --- --- --- --- --- --- --- Y
 $ $ $ $ $ $ $ $ $ $ $ $ $ $ $ |
- - - - - - - - --- --- --- --- --- --- --- |___ X
finer coarser Surface 2

 $ sign indicates the Node-To-Node Contact Element between the Nodes of Surface 1 and 2 respectively. If you observe the mesh variation along X direction, it has varied from Finer to coarser. In such situations, use of a uniform Kn value for all the N-T-N contact elements could lead to un-even contact pressures. It is advisable to specify different values of Kn. If this step was not taken care of, then the finely meshed portion will experience more stiffness compared to the coarsely meshed portion. To avoid these issues, its recommended practice to use the same edge length between the two surfaces 1 & 2.

Return to Top

41. What are the guidelines to estimate FKN for a contact Analysis.

For bulky contact, where the two are solid bodies FKN = 0.1 to 10 ---> Factor of E For contact between two slender bodies ( thin / bending dominated structures) FKN = 0.01 to 1 ---> Factor of E Its always advised to start with a lower value of FKN and proceed later with higher values. The default setting in Ansys is 1, irrespective of what kind of bodies are participating are getting in Contact.

Return to Top

42. When two different material (say Steel and Aluminum) are in Contact, which material's E should be considered for evaluating FKN

E of the softer material be always considered for estimating FKN. In this case prefer E of Aluminum.

Return to Top

43. How to specify Sticking and Sliding conditions for Contact between two bodies?

'Mu' - Friction coefficient and TAUMAX are the two inputs user needs to specify. If Ft >= Mu*Fn where Fn --> Normal Force & Ft --> Tangential Force, the bodies slide relative to each opther and the two contacting bodies experince a Shear force of TAUMAX. Sticking happens when Ft < Mu*Fn

Return to Top

44. How to estimate TAUMAX?

TAUMAX = (Von Mises Yield Stress/1.732) This is an empirical formula

Return to Top

45. I have Higher order elements (with mid-side nodes) on the two contacting surfaces & I want to analyse the problem using NTN Contact. Can I create NTN Contact between the mid-side Nodes?

Due to the uneven nature of the kinematically consistent reaction forces at the nodes of midside-noded elements, NTN contact should NOT be applied to mid-side nodes. In effect, usage of NTN implies that only lower order elements be used for underlying mesh of contacting parts.

Return to Top

46. While editing the real constants of a Contact element, like FKN can negative values be entered?

In the Real Constant menu, a negative value indicates an absolute value; and a positive is considered as a factor. So if FKN was specified as 0.1, its considered as 0.1*E Else, if FKN was specified as -2e10 then the value of FKN for the analysis is -2e10

Return to Top

47. How does FTOLN affect convergence & Accuracy of results?

After FKN, FTOLN is the next parameter that affects both convergence & accuracy. Its usually known as Penetration Tolerance(TOLN) This is a factor of the depth of the underlying element. If the underlying elements depth was [h], and if FTOLN is specified as 0.1 (default value), a penetration of (0.1*h) is allowed. If this value was exceeded during the solution, then solution does not converge. Its aborted. In effect, this value can be treated as the Maximum allowable penetration. Setting too small a value can also affect in the form of excessive iterations or non-convergence.

Return to Top

48. How and where is contact detected?

For STS elements, only the Target elements can penetrate into the Contact Elements and NOT vice-versa. Gauss-Integration points on the Contact Surface act as the Contact detection points. This is the default setting and is recommended for most cases. The Newton-Cotes/Lobatto nodal integration scheme, uses the Nodes of the Contact elements as Contact Detection points.

Return to Top

49. There are several Contact Surface behaviour options on the Contact Wizard. What does each one of them do/describe?

STANDARD: Normal contact closing and opening behavior, with normal sticking/sliding friction behavior.

ROUGH: Normal contact closing and opening behavior, but no sliding can occur. The surfaces are assumed to be so rough that there is infinite Friction and there can be no relative Sliding.

BONDED: Target and contact surfaces are assumed to get

GLUED once contact is established.

BONDED CONTACT (always): Any contact detection points initially inside the pinball region or that come into contact are bonded for the remainder of the analysis. This contact typically can be used to "ADD" two meshes in a Assembly analysis where two parts have different meshes. A linear Static analysis can also be solved with this contact. Though ansys would prompt for nonlinear analysis(due to presence of contact elements) a single iteration is enough

BONDED CONTACT (initial contact): Bonds surfaces ONLY in initial contact, initially open surfaces will remain open.

NO SEPERATION: Target and contact surfaces are tied once contact is established (sliding is permitted).

NO SEPERATION (always): Any contact detection points initially inside the pinball region or that come into contact are tied in the normal direction (sliding is permitted).

Return to Top

50. How should I simulate interference? Between two parts there exists both interference as well as Gap between their surfaces? Using STS Contact element, what factors need to be adjusted/set ?

In most of the FE models, the exact interfernce cannot be modeled with all that accuracy. Hence there exists a parameter called CNOF which can be tweaked, either to set a interfernce or a Gap. A positive value of CNOF is considered as INTERFERENCE, while a negative value of CNOF is considered as GAP. Using CNOF will either move the Contact Surface inwards/outwards for the Analysis. The Target surface will not be moved. So, if you are modeling contact btw two flexible bodies... please note that the surface designated as Target will not be offset. If the model contains initial geometric penetration+CNOF, it is recommended to set the initial interference option to "include with ramped effects". If this setting was not set, there is every chance that due to initial penetrations, the contact forces will be stepped (not ramped) to a huge value and there is every possibility for a un-converged solution. If both GAP and Interference exists in the model, different CNOF values will have to be specified between the various surfaces of the Parts.

Return to Top

51. RIGID body motion error. I have the FE model with well defined constraints. Yet I see this error in the very beginning of the Solution. How can I avoid this error?

A rigid body motion can occur just before contact is established between two parts. You may use a displacement so as to initiate contact in the first load step. In the second load step delete this displacement, and apply the reaction force obtained from previous load step. This will switch your problem from displacement controlled problem to a force controlled problem. In the subsequent load step(3) continue with the load history. Weak springs that are connected to Ground can be used to control Rigid body motions. The Spring stiffness should be very small compared to the stiffness of the system. Though, the spring may deform... its of no concern. The above two techniques involve some experimentation from the user. Also, they cannot be used in all kinds of problems. They are restricted. Ansys provides 3 parameters to control RIGID BODY MOTION 1. ICONT 2. PMIN-PMAX and 3. CNOF 1. ICONT: This is a real-constant value, which specified a zone/band around thesurface of Target Elements. Any contact points lying within this Zone, are shifted to the target surface. Ansys uses a small default value of ICONT if not specified by the user. This value should not be set to ZERO. If set to Zero, Ansys uses a default value. To turn it OFF specify a a very small value liek 1e-20. If there is a Gap of say 0.25mm between the Target and the contact surface & this happens to be the first place where contact happens, then specify ICONT as 10% more than this Gap. ICONT = 0.275mm Please note that ICONT is not any factor, its a constant value unlike other parameters PMIN-PMAX: Use real constants PMIN and PMAX to specify an initial allowable penetration range. The Target surface shall be moved into the Contact Surface and made to lie within PMIN-PMAX. This is acheived with a few interations before the load history comes into effect. By using this feature, the gaps lying between Contact and Target Surfaces will be converted into a initial closed contact. If any of the nodes on the Target surface had constraints, then that particular node will not be moved in the constrained direction. 3. CNOF: [ see the previous FAQ. ]

Return to Top

52. In a Flexible-Flexible body contact, Why should the surface with finer Mesh be designated as Contact Surface, and the other surface (with coarse mesh) be designated as Target?

The Finer mesh will have more contact detection points. This will help the analysis solve better. Please note that elements/nodes on Target surface do not detect contact. In a flexible-flexible body contact, the choice of the target and contact surface can cause a different amount of penetration and thus affect the solution accuracy. Choose that surface which tends to move towards the other as the Contact Surface. (Assuming that both surfaces have same mesh density & have relatively small difference in their structural stiffness)

Return to Top

53. Guidelines to choose Target/Contact Surface

  1. If a convex surface comes into contact with a flat or concave surface, the flat or concave surface should be the target surface.
  2. If one surface has a coarse mesh and the other a fine mesh, the surface with the coarse mesh should be the target surface.
  3. If one surface is stiffer than the other, the stiffer surface should be the target surface.
  4. If one surface is higher order and the other is lower order, the lower order surface should be the target surface.
  5. If one surface is larger than the other, the larger surface should be the target surface

Return to Top

54. What is Pinball Region ? What does it affect? What is its purpose in Contact Analysis?

Pinball region (PINB) affects the contact status determination. This Pinball Region is a circle (2D) or sphere(3D) around the Contact element. This Region helps figure out how "far" and "near" regions around the Contact element. If l ==> depth of underlying element, in Rigid-to-FLex Contact, the Pinball region is 4*l. For flex-flex contact, the Pinball Region is 2*l. The position and motion of a contact element relative to its associated target surface determines the contact element status. ANSYS monitors each contact element and assigns a status:

STAT = 0 Open far-field contact

STAT = 1 Open near-field contact

STAT = 2 Sliding contact

STAT = 3 Sticking contact

A contact element is considered to be in near-field contact when its contact element enters a pinball region, which is centered on the integration point of the contact element.

Return to Top

55. What type of Contact is best suited to simulate Interference fit kind of problems? NTN type of Contact is best suited to simulate Interference Fit kind of problems. Most interference problems have negligible relative sliding deformation.

NTN Contact is the least expensive in terms of solution times when compared to STS and NTS type of contact. Also, convergence issues are lesser.

Return to Top

56. For NTN elements, how should the axis of NTN element be oriented? (I-J orientation of element)

Typically the I-J direction should be perpendicular to the contact surfaces. If the angles are not perpendicular undesired tangential responses will be generated between the Contact surfaces.

 

Return to Top

XANSYS FAQ (Frequently Asked Questions)