Ansys 9 and Contact 1

[cnuk]

I am trying to do the example at:

http://www.mece.ualberta.ca/tutorials/ansys/AT/Contact/Contact.html

Using Ansys 9. The first thing I notice is that I do not have element CONTAC48 available. The next thing I notice is that when I go through the contact wizard and setup a contact pair (symmetric or not, various types:surf-surf,node-surf, etc) it does not seem to be taken into account by Ansys during the solution. Solve seems to run fine, but I have result scaling set properly and the top beam still penetrates the bottom.

Can anyone tell me what kind of contact pair I should be setting up for this problem? Anything else I should be looking for? I am new to contact and this seems like as simple an example as it gets.

Also, has anyone else seen the picker dialog get lost behind the other windows when using the contact wizard? Sure seems to happen a lot on my machine.

Thank You

 

[Drej]

> The first thing I notice is that I do not have element CONTAC48 available.

This element is obsolete in V8+.

> The next thing I notice is that when I go through the contact wizard and setup a contact pair (symmetric or not, various types:surf-surf,node-surf, etc) it does not seem to be taken into account by Ansys during the solution.

If you didn't use contac48, which contact element(s) did you use? How do you know that it "does not seem to be taken into account by ANSYS"?

> Solve seems to run fine, but I have result scaling set properly and the top beam still penetrates the bottom.

You need to check your contact status before the solve. Issue the CNCHECK command and read very carefully the information in the dialogue box. We can then continue to sort your contact problem(s) out.

> Also, has anyone else seen the picker dialog get lost behind the other windows when using the contact wizard? Sure seems to happen a lot on my machine.

Yes. This is a characteristic ANSYS "feature". To the right of the command input line in the main ANSYS GUI, there is a button which looks like a blue "I". This is the "raise hidden" button, which if you press it will bring all widgets (as the dialogue boxes are called) to the front.

Cheers,

-- drej --

 

[ProtoformX]

> it does not seem to be taken into account by Ansys during the solution.

I had the same problem at first. I think you need to select the contact elements prior to running the solution. Try clicking "select everything" from the pulldown menu or issue the ALLSEL command. This solved my problem.

 

[cnuk]

I am currently using PLANE42 elements, then using the contact manager with a symmetric surface-to-surface contact. I selected the line on each body that could come into contact with the other (bottom line on top beam, top line on bottom beam). After the contact wizard is complete, I check and see that TARGE169 and CONTA172 elements were used and two contact pairs were created (symmetric contact).

I guess I think I know that the contact elements are not taken into account because when I review the results, scaled 1 to 1 the top beam almost passes through the bottom beam. If I look at contact pressure results nothing is highlighted in a fringe plot.

If I issue a CNCHECK, command with no options it says that no contact pairs were found for the operation. Do I need to specify options?


Hey, wait a minute. I just tried ProtoformX suggestion of doing a SELECT/EVERYTHING before running solve and guess what.....THE CONTACT WORKED!!!

So, why do I have to do a select everything?? Nothing I've read mentions anything like this

 

[Drej]

> So, why do I have to do a select everything?? Nothing I've read mentions anything like this

Because ANSYS will only solve for the currently selected elements. If you only select one element in your model, this is the only element that will be solved for. Try learning about ANSYS select logic, starting with the #SEL series of commands. Furthermore, select everything and then issue the CNCHECK command again, then post the resulting information.

 

[ProtoformX]

Glad I can help someone for a change.

 

[cnuk]

CNCHECK dialog initially says: "All 2 selected contact pairs are initially open. Rigid body motion may occur in any portion of the model held in place solely by contact elements".

The the CNCHECK command output reads:

*** NOTE *** CP = 2.469 TIME= 10:55:26
Symmetric Deformable- deformable contact pair identified by real
constant set 3 and contact element type 3 has been set up. The
companion pair has real constant set ID 4. Both pairs should have the
same behavior.

*** WARNING *** CP = 2.469 TIME= 10:55:26
ANSYS has found the contact pairs have similar mesh patterns which can
cause overconstraint. You may deactivate the current pair and keep
its companion pair.
Contact algorithm: Augmented Lagrange method
Contact detection at: Gauss integration point
Default contact stiffness factor FKN 1.0000
The resulting contact stiffness 0.20000E+07
Default penetration tolerance factor FTOLN 0.10000
The resulting penetration tolerance 0.20000
Frictionless contact pair is defined
Update contact stiffness for each sub-load step
Average contact surface length 2.0000
Average contact pair depth 2.0000
Default pinball region factor PINB 1.0000
The resulting pinball region 2.0000
*WARNING*: Initial penetration is included.

*** NOTE *** CP = 2.469 TIME= 10:55:26
No contact was detected for this contact pair.
****************************************


*** NOTE *** CP = 2.469 TIME= 10:55:26
Symmetric Deformable- deformable contact pair identified by real
constant set 4 and contact element type 5 has been set up. The
companion pair has real constant set ID 3. Both pairs should have the
same behavior.
For asymmetric contact analysis, you may keep the current pair and
deactivate its companion pair.
Contact algorithm: Augmented Lagrange method
Contact detection at: Gauss integration point
Default contact stiffness factor FKN 1.0000
The resulting contact stiffness 0.20000E+07
Default penetration tolerance factor FTOLN 0.10000
The resulting penetration tolerance 0.20000
Frictionless contact pair is defined
Update contact stiffness for each sub-load step
Average contact surface length 2.0000
Average contact pair depth 2.0000
Default pinball region factor PINB 1.0000
The resulting pinball region 2.0000
*WARNING*: Initial penetration is included.

*** NOTE *** CP = 2.469 TIME= 10:55:26
No contact was detected for this contact pair.
****************************************


*** WARNING *** CP = 2.469 TIME= 10:55:26
All selected contact pairs are initially open. Rigid body motion can
occur. You may use auto CNOF/ICONT by setting KEYOPT(5) to close
small gaps.

2 CONTACT PAIRS ARE SELECTED
CONTACT PAIR HAVING REAL ID = 3 IS INITIALLY OPEN
CONTACT PAIR HAVING REAL ID = 4 IS INITIALLY OPEN

Kind of greek to me. I see warnings but no errors and I don't know how serious the warnings are.

Thanks again!