I have 2 touching and trimmed C-profiles that I want to mesh with midplane mesh. But if I create the mesh there's always a gap in the corner between these two parts (something like a chamfer on both of them). If I try to mesh only a single part, Simulation Mechanical creates the "chamfer" as well (please see the pictures attached). Shorter sides of C-profiles has different thickness than the longer side. I'm not sure whether this is a feature or a bug or if I'm doing something wrong. Simulation type is Static Stress with Linear Mat. Model. I use Autodesk Simulation Mechanical 2015.
Could you post any advice?
Solved! Go to Solution.
I think the issue is with the midplane meshing process, not with your process. If you think about where the midplanes of the bottom (long side?) of the c-channels are, they won't necessarily meet up at that corner. I don't know if you're c-channel CAD models have their 45 degree chamfer just to the c-channel floors or all the way to the bottom edge of the floors. However, in either case I can see how the mesher would have problems with that.
There are several ways to fix that. The easiest is probably to grab the lines along one c-channel "floating" edge and perform a move with "move ends" selected. You can enter the vector distance to move so that the edge is located where it needs to be. Then select the lines along the other c-channel edge and move them to meet the other c-channel edge.
Hope this helps.
Sorry for my very late response, I was quite busy to take a closer look at your proposed solution. Although there is not a 45 degree angle between my c-channels, I don't think this should be a problem for the mesher because of the same thickness of both of bottom sides (see the picture attached).
I tried to move the edge nodes as you proposed but I encountered some problems. If I move the nodes, Sim. Mech. tells me that I have to start solid meshing manually for the parts - but I want midplane mesh (please see the second picture attached)... When I run the simulation, it prematurely ends with an error. Therefore I don't know how to run the simulation with manually modified mesh... Do you (or anybody else) have any suggestions?
And one more thing... Even when I try to mesh a single c-channel part only, still there's the "chamfer" at the both ends of the c-channel. M.
I think the chamfer that shows up is due to ASIM having difficulty with the angle on the end of your channel. Look at the midplanes with lines.png file. I have drawn a line in pink where ASIM believes the midplane is. Notice that it is not extending the midplane line of each channel to meet the other channel. It just finds the midplane of each part and leaves it as is.
The way to move the edges so you have the part you want is to set "select lines", grab all the lines along one edge of your floating chamfer, perform a "move or copy" with "move ends" selected. You can then select the correct distance you want the edge to move. Do the same with the edge lines on the other channel. For that move you can just select the vector and snap from the edge you want to move to the other one you've already moved. That should close your c-channel assembly correctly.
When you make the manual moves, you will get the warning that you've see already, but you can ignore that. It has nothing to do with solid or midplane meshing. Just make sure that when you do the manual moves you don't re-mesh the model. If you do, it will revert to the original configuration. It is best to do the manual moves once you've completed all the automeshing. I went through this process myself on a sample model, and the model ran just fine.
I have included a picture of the edge move process from my sample model.
Sorry again for my very late response. That was what I needed to know - to move the edge using the "move or copy" command with "move ends" option. Previously I used the Move (Point Move) command and therefore I was forced to remesh the model.
OK, the bad news are here... The simulation still fails with some nice messages, see below:
**** DYNAMIC NODAL LOADS
ERROR - Unable to process model.
Error occurred with module: C:\Program Files\Autodesk\Simulation 2015\srunx.exe
**** BEGIN NODAL DATA INPUT
ERROR - Unable to process model.
The model contains errors due to geometry problems.
In working on FEM file for a FEA model
Terminal Error: FEM2ESH#108
make sure it is mid-plane mesh (varying thickness?) 6
Nevertheless, I think we can skip this topic...
My colleague Pat made a post a few months back with a list of all the FEM2ESH errors that have been encountered by technical support over the years, here is the information available on FEM2ESH#108.
Error Message: Terminal Error: FEM2ESH#108, FEMAPI#1
Decoding Processor: FEM2ESH Error Number: 108
Decoding Module: FEMAPI Part Number: 1
Error Description and Proposed Solution:
Define the thickness after mid-plane meshing a part.
Was the thickness for all parts with a midplane mesh define beforehand?
If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!
I think I have found what causes the error message. It is because of the different thickness of the c-channel bottom and side walls. For example, if the c-channel bottom will have the thickness of 10 mm and sides will have the thickness of 6 mm, Simulation Mechanical is not able to handle this situation after the changes to the mesh have been made manually by moving the edge lines of the midplane mesh. If the c-channel has the same thickness on its bottom as well as on its sides, I can manually move the edge of mesh and Simulation Mechanical is able to run the simulation correctly again. Please, take a look at some pictures attached.
If I think about it further, does this mean that midplane meshing should not be used for geometry with different thickness? Although the thickness of the c-channel is distributed uniformly across the part (same at the bottom and same on the side walls...).