Separation Contact - Load Not Transferring

[travis.potier]

I have an analysis I'm trying to complete which requires two components to slide against each other making one move to close a specified gap. The separation contact is the most realistic surface contact for this analysis, however, the load will not transfer through the separation contact face. I've run it with bonded contacts to verify it's a contact issue. Bonded contact does transfer the load, but obviously does not give me realistic results. Has anyone faced this problem before and have recommended solutions?

[John_Holtz]

Hi @travis.potier 

Out of curiosity, what are the results that make you think the separation contact is not working? What type of analysis are you using?

If you are using linear static stress and looking at the deformed shape to determine if it is working or not, you need to set the displacement scale to the actual value of 1. If you magnify the displaced shape (which you usually do in a linear static analysis so that you can see the small displacement), then you are magnifying the effects of the gap between the parts, too.

See Separation contact does not prevent parts from penetrating in Autodesk Nastran In-CAD.

[travis.potier]

The reason I believe it is not transferring the load is that one of the contacting components show 0 stress and deflection while the component that is loaded (has a pressure applied to it) has both stress and deflection. Note this is not just from the display and having it scaled properly, there is literally no stress/deflection in the secondary component. The face on the loaded component that is in contact with the secondary component also has 0 deflection. The secondary part also comes in contact with a 3rd component. There is 0 stress and 0 deflection at that contact point, indicating no load being transferred into the second component. When I switched to bonded contacts, all 3 components then had resulting stress and deflection as expected.

This was in a linear static analysis. Once I get a completed linear static analysis with "expected" results (confirming all conditions have been applied appropriately), I'll switch to a nonlinear static analysis.

[John_Holtz]

I do not have any ideas at the moment. Would you be able to provide the model? If so, zip the part (.ipt files) and assembly (.iam files) together and attach it to the forum. (See Roelof's video How to create a Pack and Go with Inventor for additional instructions on zipping the model.)

If you cannot provide the model, then we need a lot of details, such as:

1. What type of elements? Solid or shell or both?
2. What is the separation between the parts?
3. What is the mesh size around the contact location?
4. What contact are you using? Auto, manual, or solver?
5. What are the settings for the contact, especially the maximum activation distance?
6. What is the displacement of the loaded part, at the location where contact should occur?

[travis.potier]

Hi John,

I'm not able to share the model, but I can attach screenshots and answer your questions. Also, I did some more playing around with the model and have gathered more information. I've attached 3 screen shots. One of the area in concern unloaded just for reference, then two other with different loads (pressures) applied. In the two loaded screenshots, the displacement scale is set to actual (1).

The picture showing the larger displacement is with 3000 psi applied. The picture with the smaller displacement is with 4000 psi. There definitely shouldn't be a smaller displacement when a larger pressure is applied. Based on this, it appears the problem is driven by closing the gaps shown (which is the whole point of my analysis - trying to determine what it takes to close the gaps and material effects thereof). The model fails when the gaps fully close; I just don't know how the displayed results come to be.

Here's the answers to your questions:

1. What type of elements? Solid or shell or both?
   1. Solid
2. What is the separation between the parts?
   1. There are a total of 4 components as shown in the picture. As can be seen, some are initially in contact, others aren't.
3. What is the mesh size around the contact location?
   1. 0.01 via mesh control. I will try different mesh configurations
4. What contact are you using? Auto, manual, or solver?
   1. Manual
5. What are the settings for the contact, especially the maximum activation distance?
   1. Separation type - symmetric
   2. Stiffness factor = 1
   3. Coefficient of friction = 0.13 (considered normal for metal-to-metal contact in my industry)
      1. I have tried  no friction (coefficient = 0) as well
   4. Max activation distance: for those initially in contact it is set to auto; for those with initial gaps it is set to the distance in the initial gap (0.015" for one set and 0.0075" for another)
6. What is the displacement of the loaded part, at the location where contact should occur?
   1. Two screenshots attached show total displacement

[John_Holtz · Accepted solution]

Hi @travis.potier 

It looks like one of the models has springs, presumably to make the part(s) statically stable. That will be necessary in a linear static analysis (even a nonlinear static analysis) when the parts have gaps. In the initial position, there is nothing holding the part with the load, so it can move an infinite distance in the static analysis. Whether the analysis can recover from that condition is debatable.

Here are some ideas to try:

1. Make sure each part is statically stable without depending on the contact. Add additional springs to stabilize the parts as necessary. (As a starting point, try a spring stiffness that allows the parts to move 10X the gap when the full pressure is applied.)
2. It appears that friction is not supported in linear static stress. Set it to 0 if you continue to use linear static stress. Otherwise, use nonlinear static stress to include friction.
3. The alternative to a static analysis (and the problem with stability and gaps) is to perform a nonlinear transient stress.

[travis.potier]

Hi @John_Holtz ,

You are correct. Each non-fixed component has 6 springs (2 for each direction, 1 in the positive and 1 in the negative) with the end of each spring being fixed. I'll look at implementing your suggestions below and see how it goes. Thanks for all the input!

Travis

[John_Holtz · Accepted solution]

Hi @travis.potier 

(Travis provided the model through Technical Support, but I am replying to the forum so that others can learn what I found out. Sorry that others cannot look at the confidential model, other than images.)

I worked with the nonlinear transient model that you provided. Because of the long run time, I reduced the model to just the "Pin" and "BUP" parts. (Literally the two parts shown in the image below.) Previously, the contact between the BUP and Pin was not being detected.

1. I set the Maximum Activation Distance to 0.04 inch. This accounts for the 0.015 inch gap and the mesh size, and allows some sliding of the surfaces if that occurs.
2. In the transient analysis, I was able to see the BUP move to close the gap, come into contact with the Pin as the load was being ramped up, sit in contact for a few time steps, and then "push" through and fly off into space! 
3. Probably what happens is this. In Nastran contact, there is no force when the parts are 0 inches apart. In order to develop a contact force, the parts have to (mathematically) penetrate each other. If the penetration is "too large", the solver decides that it is better to remove the contact. I think this is what happens in this model.
4. I think the best solution is to increase the contact stiffness from 1 to 10. That worked in the 2-part transient model.
5. The alternative is to adjust the contact "Advanced Options > Maximum allowable penetration". In general, a value about 10% of the mesh size (at the contact) is acceptable. (Smaller values are better to limit the penetration.) I did not try this option. 
6. The other thing I noticed is related to the springs. The spring stiffness K1 is in the "X" direction regardless of how the springs are oriented. Since you are using the springs to provide some stability and are not trying to replicate a real stiffness, the safe thing to do is click the "Advanced Options" and enter the same spring stiffness for K1, K2, and K3. That will provide a resistance force in "X", "Y", and "Z", where the directions really depend on the coordinate system assigned to the springs. See How to enter spring stiffness in Nastran .

P.S. The other possibility is this. You may need to increase the contact stiffness at the other areas where the BUP contacts the other parts. When the other parts are included in the analysis, the BUP makes contact with them first. What could happen is that the BUP does not contact the pin until the BUP "breaks through" the other parts. The BUP could accelerate so fast that the "collision" with the pin is missed by the analysis.

[John_Holtz]

Hi @travis.potier 

I wanted to follow-up to see if you tried changing the contact stiffnesses (or other settings) and what the outcome was. Are the parts still passing through?

[travis.potier]

Hi John,

For some reason I never got a notification of your post. I was logging on to "accept solution" when I saw it. I've been able to get the parts to not pass through each other by using the contact stiffness and allowable penetration techniques you specified.

I'm still having trouble getting completed analyses, but I'll close this post out as it's primary question has been answered. I may make more posts as I come to dead ends again.

Thanks for all of your help.

Travis