Simulation Mechanical Forums (Read-Only)
Welcome to Autodesk’s Simulation Mechanical Forums. Share your knowledge, ask questions, and explore popular Simulation Mechanical topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Initial Gaps and Contact

9 REPLIES 9
Reply
Message 1 of 10
BEC_Kevin
875 Views, 9 Replies

Initial Gaps and Contact

I am having some trouble getting gap elements to work. I have never used these before, so I am after a little guidance.

 

This is a linear structural analysis of a small assembly. Initialy, I have a gap of about .125" that eventually hits a surface. To make the matter worse, it is sort of like a square rotating inside a box, so the contact is edge to a surface. I have tried defining some gap elements in the assembly but I could not get a solution after 2 hours of run time. WIthout the gap elements, the "square" is just rotating through the "box".Would it be recommended that I plan to allow the analysis to run longer than 2 hours? Perhaps overnight?

 

Any tips or thoughts would be greatly appriciated! Thank you in advance.

9 REPLIES 9
Message 2 of 10
S.LI
in reply to: BEC_Kevin

did you try to set contacts between "square" and "box" instead of gap elements?

Are you using ALgor MES? 

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 3 of 10
John_Holtz
in reply to: S.LI

I presume that a "linear structural analysis" means that the analysis type is Linear Static Stress. If this is correct, then the hand-drawn gap elements are the only option, and these can only connect nodes on the square to nodes on the surface. (This is true of all types of contact in linear stress, but Mechanical Event Simulation -- MES -- has true node to surface contact.)

 

My guess is that the model is not statically stable without the gap elements. That is, if you deactivate the gap elements, is every part in the assembly statically stable? No parts are free to translate or rotate? It could be that the model is too unstable and the software keeps searching for a solution.

 

If you have not already done so, I suggest reviewing the suggestions under the "Help > Contents > Autodesk Algor Simulation > Setting Up and Performing the Analysis > Setting Up Part 3 > Performing the Analysis > Performing A Linear Analysis > Performing Analyses with Gap Elements".

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉
Message 4 of 10
BEC_Kevin
in reply to: S.LI

I did set contact surfaces, I tried both surface contact, and edge contact, neither had worked. The parts just go through one another. Not sure what "MES" is? I am new to the software. I have been trained FEA on ANSYS, so I am still getting used to the interface change.

 

A little more info, I am pulling the model in from Solid Edge 3D modeling. I save the file as a .STEP file, and open that in Algor. It seems to work better than going straight from SE.

 

My research keeps directing me toward gap elements. I just am not sure how to apply the elements in this situation however. Having a 2+ hour solution for trial and error methods is a little tough to justify to the boss! haha.  Thank you again for the help!

Message 5 of 10
BEC_Kevin
in reply to: John_Holtz

The parts are statically stable without the gap elements. In that attachment, I have hidden a few parts. It does solve, but the parts go through one another, which is what I am trying to resolve. Once the edges come in contact with the surrounding "box", they need to transmit forces.

Message 6 of 10
S.LI
in reply to: BEC_Kevin

I think contact should be the way for your model.

 

 

Can you share your model here?

it's the best way for us to help you.

 

If not, could you share your log file? log files are some files called ds.alg or ds.lg.

 

 

 

Thanks.

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 7 of 10
BEC_Kevin
in reply to: S.LI

I would rather not share the actual model on here, no offence. I can provide screen shots and information of the area in question. I think the biggest questions I have are just about the use of gap elements. I feel that the correct use of these elements will get me to my solution.

 

I have successfully solved the model with a lighter load case. The parts rotate about that pin, but there is not contact. Since then, I had desired to see what will happen if the loading increases, and those surfaces come in contact, how the forces/displacements distrubute. The previous model (without contact) solved in 15 minutes. With the introduction of gap elements, should I expect such a long solution, in the order of hours?

 

Message 8 of 10
S.LI
in reply to: BEC_Kevin

The reason why I asked log file is to identify your analysis type, LSS or MES. For different analysis type, the model settings and behavior could be totally different.

 

LSS is not suit for your model, I guess, since there are big motions here.

 

I just assume you are using MES. It's very possible to take several hours or days to solve a MES model, especially with surface or part contacts. If the simulation runs well (according to the log on fly), I guess you can give it more time.

 

 

----------------------------------------------------------------------------------------------
If this response answers your concern, please mark it as "solved".
Message 9 of 10
BEC_Kevin
in reply to: BEC_Kevin

I do not have a license for MES. It looks that I am asking a little much for my linear analysis then... I take it that with the linear solutions, gap elements require direct node-to-node contact. This, I do not have. Rather, the nodes are contacting on the surface of another part (between nodes), which is causing for an indefinate solution. The gap elements can never close.

 

Thank you for the assistance! Its very much appriciated, and I will post back if I can get anything to work out.

Message 10 of 10
John_Holtz
in reply to: BEC_Kevin

Hi,

 

In linear stress, the "Surface Contact" and "Edge Contact" only work when there is no gap between the surfaces, so I can confirm that those will not work in your case. When you have a gap between the parts, the hand-drawn gap elements are the only option (in linear stress).

 

Hopefully the hole and pin that it pivots about has no gap so that you can use the "Surface Contact" on that interface. If it does have a gap, I suggest that you either change the CAD model or change the "Mesh > Model Mesh Settings > Options > Model > On-surface tolerance based on > Absolute length dimension" and enter a dimension slightly larger than the gap between the hole and pin.

 

Here are some other tips.

 

1) In order to use the hand-drawn gap elements, you will need nodes on the box that are directly or straight across from the nodes on the end of the square. You can force nodes to be located at specific coordinates on the box by adding Construction Vertices. ("Autodesk Algor Simulation > Meshing Overview > Mesh Overview > Meshing CAD Solid Models > Construction Vertices - Seed Points") What I would do is this:

   a) mesh the model

   b) draw lines on an unused part number that extend from the end of the square, are perpendicular to the side of the box, and end in the plane of the side. These will become the gap elements.

   c) hide all parts except for the square and new gap elements.

   d) add construction vertices to the box end of the gap elements.

   e) remesh the model. This should create nodes on the box that coincide with the nodes on the gap elements.

   f) define the Element Type for the lines as gap elements.

   g) define the Element Definition for the gap elements as type "Compression with Gap".

 

2) Run the analysis. The reason it takes longer is because the solution becomes iterative. We cannot calculate the answer until we know which points are in contact, and we do not know which points are in contact until we calculate the answer!

 

3) When looking at the results, check for negative forces (compression force) in the hand-drawn gap elements. "Results > Element Forces and Moments > Axial Force".

 

4) The displacements in linear stress are usually so small that the displaced shape needs to be exaggerated by some large amount like hundreds or thousands of times. You need to change that scale to 1; otherwise the displaced shape will "look wrong". (Think of it. If the square moves 1/8 inch and you exaggerate that by a factor of 8, it will look as if it moved 1 inch.) So, change the "Results Options > Displaced Model Options > As an Absolute Value" and "Scale Factor" = 1.

 

Good luck.

 



John Holtz, P.E.

Global Product Support
Autodesk, Inc.


If not provided already, be sure to indicate the version of Inventor Nastran you are using!

"The knowledge you seek is at knowledge.autodesk.com" - Confucius 😉

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report