Phantom Displacement Constraints

[Anonymous]

I have a beam/plate model that has numerous parts suppressed and other parts merged into it from Inventor .ipt files. I ran the analysis and the results appeared to have some extra displacement constraints. I exported the model as an Ansys .cdb file and displacement constraints are on the locations that I applied them to but also at four other nodes. I tried to inquire reaction results on those nodes but the node number does not exist in the model. Is there a way to rebuild the database/model or what other options do I have ??? The attached image shows that constraints are resulting in the tube bending upwards when it should be bending downwards.

[S.LI]

Could I ask several questions about your model?

1.) what's the ASIM version?

2.) what's the analysis type, LSS, MES or others?

3.) Is the reaction output enabled for this model, such as reaction force, moment?

4.) Is this displacement constraint or prescribed displacement?

5.) Can you see these extract constraints in Results tab (kinds of arrows)?

Thanks.

[Anonymous]

1. Autodesk Simulation Mechanical 2012 Buikd 2012.01.00.0017.

2. Analysis type is LSS.

3. The reaction output is enabled in the output file.

4. This is displacement constraints of zero at the four nodes (all translations and rotations).

5. The extra constraints are not visible in either the FEA Editor or the Results environment but they are making the results useless to me.

I hope this helps. The database is quite large or I would send it to you. I will see how small I can get it.

[S.LI]

Could these points be k-nodes for beam elements?

In order to define beam orientations, ASIM automatically generates several k-nodes, and they are fully constrained.

You may find more about k-node in ASIM WIKI or help.

In both FEA Editor and the file you exported, you should see coordinates for these nodes.

Do they match with each other?

Please make sure coordinates of k-nodes are large enough compared with your model size.

[S.LI]

BTW:

Could other reasons lead to the wrong results?

Or you are pretty sure it's because of extract constraints.

Thanks.

[Anonymous]

I exported the model as an Ansys file and then opened it with Simulation again. I lost some of the beam x-sections and end releases in the process but the model solves correctly now. What export format would I lose the least data in? If you would like me to send my database to you I could do that - it's 45MB.

[S.LI]

I'm not sure how importing and exporting work.

What do you mean " the model solves correctly now"? Do you get results you expect?

Maybe the mistakes in model DB already got fixed during exporting, importing, resetting etc.

[Anonymous]

The database seems to still be corrupt but by exporting it and importing it to a new model it gets around the problem. I am just about to solve the rebuilt model now with all the correct loads and constraints so I will check it out once more. I plan on submitting the problem model to Autodesk to see what they can find. I will keep you posted (pun intended).

[S.LI]

Thanks and good luck.

BTW, do you get a chance to see if the extra constraints in your export file are the k-nodes or not? I'm pretty curious on this.

Best,

[Anonymous]

How do I check that out easily in Simulation? Can I get the coordinates of the k-nodes easily? Are the k-nodes usually constrained in all DOF's?

[S.LI]

K-nodes are fully constrained.

To check them, select a beam element, right-click and pick up "Beam Orientations", you should see the following picture.

"Use Default" means code generates them at far away places. Otherwise, you should see the coordinates there.

[sunj.autodesk]

Another way to try:

Can you temporarily disable/surpress the other parts and only keep the problematic part? Try add some loads and boundary conditions on it and see whether the phantom displacment constraint still exist?

[John_Holtz]

Hi,

Actually, I am not sure that you clearly indicated where these "phantom constraints" appear in your model. From looking at your original screenshot, most of us probably assumed the item you were talking about is the circle just underneath the arrow at the top of the image. That's what I assumed.

By enlarging the image, I noticed that the circle is orange, not red. Orange circles are beam end releases. I assume that the location coincides with the location where you applied end releases in the FEA Editor. Note that the symbol appears part way between the two nodes on the beam.

[Anonymous]

Sorry to throw you off with the beam end release. I don't know where the phantom constraints are as they do not show up in the model anywhere. I spoke to Pat Tessaro this morning - he has the model and is checking through the database to determine what is really happening. I will be sure and let all know what he finds out. Thanks for all your input.

[Anonymous · Accepted solution]

The model had some very poorly shaped elements that were created due to the presence of construction points. The poorly shaped elements resulted in a large variance of stiffness and an ill-conditioned matrix. The only clue was a warning message that the stiffness ratio exceeded a predetermined warning value.

[S.LI]

Thanks for your update.