The following are two common reasons for this:
(1) mesh-based de-featuring of very small geometry and
(2) auto-rejection of contact with too-large of a gap.
how to solve this defeaturing problem can you tell me
Click on Mesh and in the Details window, Automatic Mesh Defeaturing is set to Yes. Change that to No.
The reason is that you have a contact defined on that face and that face doesn't have any mesh since it defeatured away. Check the defeaturing tolerance, set the value such so that mesh can walk over unnecessary features and avoid higher mesh count but smaller than the features you want to capture properly like bolt holes, fillets etc. If you have few contacts, you can do visual inspection for contact with no mesh.
i changed automatic mesh defeaturing to no , but the result was same
Set the variable "contactAllowEmpty" to 1 in order to allow the solution to proceed with an ANSYS warning which can be used to identify the offending contact pair(s) by reading the Solution Output.
@peteroznewman I am encountering similar problem. The message displayed is "At least one contact pair or remote load has no elements in it. This may be due to mesh based defeaturing of the geometry. You may select the offending object via RMB on this warning in the Messages window."
I implemented the suggestions that you have mentioned above regarding the use if variable. However the problem still persist. I deactivated the contacts and checked again. It still gives the error. I also deactivated remote loads, and it still didn't work.
A previous iteration of the same model worked perfectly fine.
Start with the previous iteration and update it with the changes needed to get to the current version. See if the problem returns or if you end up with a useful model.
I followed your advice but the problem still persist. Could you please look into the model? I have attached it here.
I opened your archive with ANSYS 2020 R1 but I don't know which version you are using. Please reply with the version you are using.
I notice this warning in your model.
When I follow those directions, I can find some Coordinate Systems that have lost scoping. I don't know if that has anything to do with your problem, since those are suppressed.
Later, I will go and try to solve your model in ANSYS 2020 R1 and look for the problem you reported.
@peteroznewman Hi. I am using ANSYS 2019 R2.
@peteroznewman It shows that warning message because the geometry was changed by me. The co-ordinates system were earlier defined by geometry selection. Before sending you the document, I defined the co-ordinate system using axes. Some of the co-ordinate systems are actually suppressed by me, as the they and the corresponding children are not needed for this simulation.
@peteroznewman I have found out the problem. Its very small. Some of the co-ordinate systems were not realigned by me to a proper position after making CAD changes. The remote points are placed on those respective misaligned respective co-ordinate systems with the flanges of plates scoped to the remote points. As the co-ordinate systems were placed away from it, it the flanges went out of pinball region and gave the error. I realigned the co-ordinate systems and the simulation started working again.
@AmbarNaik13 I'm glad you found the mistake. I was able to write out the input file, but it is so large and there are so many places to check that would be very difficult to find the problem.
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.