FEA error output
Here are some details for the linear static analysis error output file. Can anyone have some ideas to solve it?
*** See next message about line 451274 from file:
C:/Users/yu3/Desktop/global/global 1.1 spot.fem
"RBE2 160 44075 123456 44075"
*** ERROR # 2319 *** in the input data:
GMi # 44075 references itself recursively.
*** More of ERROR messages # 2319 were suppressed...
*** See next message about line 1006159 from file:
C:/Users/yu3/Desktop/global/global 1.1 spot.fem
"MAT1 2507632.0348091.00.35 1.05-9"
*** WARNING # 1030
Consistency requirement E=2G(1+NU) violated (by 85%).
Different values of G (either provided or inferred depending on element type)
will be used. See the Material Property Checks section of the documentation.
MAXIMUM DISK SPACE USED 1 MB"
Best Answer
-
allen_21155 said:
Yea, I get what you mean, but that existing mesh is combined mesh (both 2d and 3d are bounded together, and I don't know how to separate) and included in that 3d model component. And their geometries are now separated, so I'm thinking to remesh them individually. And I wasn't meshing that model (receiving it from others), I'm just combining several components and running the FEA on a global assembly. That attachemnt is that 3d model. If you can separate their mesh, that will help me a lot!
Ok, if you are redoing then that is fine, but you can organise elements 'by config' and select the shells only to move, they can remain 'joined' together at nodes (or even shells that are on the faces of the solids, that is ok), there is no need to 'separate' them physically
0
Altair EmployeeAnswers
-
I thought I had seen that this had been answered already but you have the same node defined as a independent and a dependent node.
0 -
Ben Buchanan said:
I thought I had seen that this had been answered already but you have the same node defined as a independent and a dependent node.
I know how to check the dependency for the rigid element, but for which tool can fix the multiple dependencies, and how to solve the 'warning# 1030' message?
0 -
allen_21155 said:
I know how to check the dependency for the rigid element, but for which tool can fix the multiple dependencies, and how to solve the 'warning# 1030' message?
Oh sorry, guess I skipped over that part when reading. Warnings will not stop it from running but to fix it you just need to change the E, G or NU on that material card so that E=2G(1+NU) is true.
1 -
Ben Buchanan said:
Oh sorry, guess I skipped over that part when reading. Warnings will not stop it from running but to fix it you just need to change the E, G or NU on that material card so that E=2G(1+NU) is true.
Hi, I switch to using the 'rigid' panel under the 1-D option, but there has another error output. Can you help me to figure out what the problem is?
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197968.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197969.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197970.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197971.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197972.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197973.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197974.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197975.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197976.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197977.
*** ERROR 14: Missing property # 5 referenced by CTRIA3 # 197978.
*** More of ERROR messages # 14 were suppressed...
*** Errors with missing, incorrect, or duplicate IDs found 9150 times.0 -
It is at it says, those listed tria elements are referencing property ID 5 and property ID 5 is not in your input deck
Do you have include files?
if are able to share your HM file I can take a look for you?
0 -
Paul Sharp_21301 said:
It is at it says, those listed tria elements are referencing property ID 5 and property ID 5 is not in your input deck
Do you have include files?
if are able to share your HM file I can take a look for you?
Sry, the file reaches the upper limit for the size of the attachment, but I can take several screenshots for you. The 'NONE' component includes the geometry of skin and the mesh for both skin and the main structure, the 'fuselage' component only includes the geometry of the main structure.
0 -
allen_21155 said:
Sry, the file reaches the upper limit for the size of the attachment, but I can take several screenshots for you. The 'NONE' component includes the geometry of skin and the mesh for both skin and the main structure, the 'fuselage' component only includes the geometry of the main structure.
Ah, ok, I think I see what has happened maybe. While you have a Prop ID 5, it is a 'PSOLID' prop (for bricks), and the elements that are being complained about in the error message are 'CTRIA3' (triangular shells) so they are looking for a 'PSHELL' prop 5 (which doesn't exist).
You can't have shells(trias) and bricks/tetras sharing a component, I can't tell from your picture, did you create a surface mesh in order to create tetras? You need to delete the shells from that component if they are no longer needed, or move them to a separate shell component with a shell property if you need to keep them
1 -
Paul Sharp_21301 said:
Ah, ok, I think I see what has happened maybe. While you have a Prop ID 5, it is a 'PSOLID' prop (for bricks), and the elements that are being complained about in the error message are 'CTRIA3' (triangular shells) so they are looking for a 'PSHELL' prop 5 (which doesn't exist).
You can't have shells(trias) and bricks/tetras sharing a component, I can't tell from your picture, did you create a surface mesh in order to create tetras? You need to delete the shells from that component if they are no longer needed, or move them to a separate shell component with a shell property if you need to keep them
Thank you for your advice. I'm trying to separate their geometry and mesh them individually.
0 -
allen_21155 said:
Thank you for your advice. I'm trying to separate their geometry and mesh them individually.
You don't need to separate the geometry or remesh anything you have already, if you have shell mesh you want to keep, you can just create a new component for it, assign it a shell property and organise your existing shell mesh into that component
0 -
Paul Sharp_21301 said:
You don't need to separate the geometry or remesh anything you have already, if you have shell mesh you want to keep, you can just create a new component for it, assign it a shell property and organise your existing shell mesh into that component
Yea, I get what you mean, but that existing mesh is combined mesh (both 2d and 3d are bounded together, and I don't know how to separate) and included in that 3d model component. And their geometries are now separated, so I'm thinking to remesh them individually. And I wasn't meshing that model (receiving it from others), I'm just combining several components and running the FEA on a global assembly. That attachemnt is that 3d model. If you can separate their mesh, that will help me a lot!
0 -
allen_21155 said:
Yea, I get what you mean, but that existing mesh is combined mesh (both 2d and 3d are bounded together, and I don't know how to separate) and included in that 3d model component. And their geometries are now separated, so I'm thinking to remesh them individually. And I wasn't meshing that model (receiving it from others), I'm just combining several components and running the FEA on a global assembly. That attachemnt is that 3d model. If you can separate their mesh, that will help me a lot!
Ok, if you are redoing then that is fine, but you can organise elements 'by config' and select the shells only to move, they can remain 'joined' together at nodes (or even shells that are on the faces of the solids, that is ok), there is no need to 'separate' them physically
0 -
Paul Sharp_21301 said:
Ok, if you are redoing then that is fine, but you can organise elements 'by config' and select the shells only to move, they can remain 'joined' together at nodes (or even shells that are on the faces of the solids, that is ok), there is no need to 'separate' them physically
That organize tool works, I use tria3 and tetra10 to separate their mesh. Thanks a lot!
0 -
Paul Sharp_21301 said:
Ok, if you are redoing then that is fine, but you can organise elements 'by config' and select the shells only to move, they can remain 'joined' together at nodes (or even shells that are on the faces of the solids, that is ok), there is no need to 'separate' them physically
Btw, do you know what's the mean by this warning message: "On TIE and FREEZE contact interfaces, 60 non-tied secondary nodes are also on the main side of the same contact, these nodes are exported in SETs"
0 -
allen_21155 said:
Btw, do you know what's the mean by this warning message: "On TIE and FREEZE contact interfaces, 60 non-tied secondary nodes are also on the main side of the same contact, these nodes are exported in SETs"
Yes, again, pretty much what it says, you have a tied or freeze contact set up, and in that, there are some nodes that are defined both in the main and secondary side of the contact (belong to shells/surfs of the main segment set and secondary node set) because a tied contact is a kinematic constraint, normally you should make sure the 2 sets (main/secondary) are exclusive of each other.
1