Dear sir
I have created a .inp file output using any2abaqus.
I oepn this file in abaqus and assign material properties.When i submitted
for analysiS following errors are occurring-
The job input file “Job-1.inp” has been submitted for analysis.
Error in job Job-1: THE DISTRIBUTING COUPLING WEIGHTS FOR COUPLING NODES LOCATED ON SURFACE ASSEMBLY_ANYBODYSURFACE SUM TO 0.0000. THIS VALUE IS TOO SMALL FOR PROPER BEHAVIOR OF THE ELEMENT.
These errors are following many number of times.I am attaching the .inp file.
Regards
Mohit
It is an interesting problem - i have not seen this one before. Could you send us a picture of how everything looks like? How many nodes is the constraint created to? What version of Abaqus do you use?
The second line defines a uniform distribution of the weights to all nodes. So it is strange that you get an error. Maybe it is something to ask the Simulia team.
Dear Sir,
When we are opening the mesh in abaqus ,mesh is opening but it give warnings which are following-
Warning: Node set name “NS_LEG_MUS_OBTURATOREXTERNUSINFERIOR2_1” is not consistent with the Abaqus/CAE naming convention. The region in question has been imported but additional usage or modification may require renaming.
Warning: Node set name “NS_LEG_MUS_OBTURATOREXTERNUSINFERIOR2_3” is not consistent with the Abaqus/CAE naming convention. The region in question has been imported but additional usage or modification may require renaming.
Warning: Node set name “NS_MUSCLESSPINELEFT_PSOASMAJOR_PML1I_TM_1” is not consistent with the Abaqus/CAE naming convention. The region in question has been imported but additional usage or modification may require renaming.
Warning: Node set name “NS_MUSCLESSPINELEFT_PSOASMAJOR_PML1I_TM_2” is not consistent with the Abaqus/CAE naming convention. The region in question has been imported but additional usage or modification may require renaming.
Warning: Node set name “NS_MUSCLESSPINELEFT_PSOASMAJOR_PML1I_TM_3” is not consistent with the Abaqus/CAE naming convention. The region in question has been imported but additional usage or modification may require renaming.
Warning: Node set name “NS_MUSCLESSPINELEFT_PSOASMAJOR_PML2I_TM_1” is not consistent with the Abaqus/CAE naming convention. The region in question has been imported but additional usage or modification may require renaming.
etc
2) When we are submitting the mesh for analysis after assigning material properties it gives error which are mentioned in last post.
Sir mesh have 35319 nodes and we are using abaqus 6.13-1 and have a licensed software.
Thanks.
These are just warnings about object naming, but they do not cause any problems.
Secondly, could you try selecting one of the constraints to visualize what is going on with the constraint itself? I did not ask for the total size of the mesh, but rather to see how many nodes are being selected for constraints. Maybe nothing is being selected due to alignment or other problems and this is why we get this error.
As a possible solution you could try to add weights manually after the line in my last post to see whether that helps or not. Please refer to the keyword reference manual (*coupling).
It is possible that the tie constraint within the influence radius cannot find any nodes. And the reasons for that would be a misalignment of the loads or something like that.
So a quick check would be to see how those constraints look like. I believe you can simply select one of them and it will be drawn in the main window.
You can open the code in the text editor, delete all loads except one, make it work using the keywords. At least i would do so.
Alternatively you can contact the Simulia team, responsible for Abaqus and ask them what exactly goes wrong and how it should be fixed. This syntax used to work for the last 5 years - maybe they could give an insight on what might be the problem.
Dear sir
i tried to solve it by manually deleting loads except one in notepad. It again showing same error. How loads and constraint looks ,we are enable to see this in abaqus. Only number of loads and constraints are showing in window but how it looks like we are enable to do this. Can we see how the loads and contraints are occurring using anybody model view?
Secondly our maintenance is expire so we are enable to contact abaqus team.
Plz give solution to us but we should do to solve this problem.
Thanks.
Consistency of Abaqus mesh and load can be easily checked if you can draw the mesh (or better the STL surface used for creating mesh) in the reference frame used to output forces from AnyBody. If you will see two bones overlap - it means the input/output are consistent.
You can also select the constraint with the right name and it should be visualized in the model view window. It should look like the ‘spider web’ picture in our tutorials: AnyBody to Abaqus tutorial.
When I mentioned to edit something manually i thought you will finish the following block:
According to the Abaqus keyword reference manual another line could be added after *Distributing, which would contain some parameters. Maybe this is something that is missing. Please read the keyword ref. manual.
Dear sir
i want to know that if i change the load values in the .xml file produced by any2abaqus and the again i generate the .inp file, i want to know that the changes which i intend to do will remain in the mesh or not?
Thanks.
CHanging the loads should not affect your mesh and material properties unless you defined them in the same file as the converter produced. TYpically the mesh is a separate file.
Regards,
Pavel
P.S. Have you managed to overcome the problem from previous posts? Do you mind sharing the solution with us? Thanks!
Dear Sir
We are still facing that problem. To overcome the problem we had did following steps-
1)I export the right femur bone from anybody modelling system to avoid misalignment problem.(we are not using own bone)
2)Then i prepare a volume mesh of that bone.
3)Then i apply loads on that bone using any2abaqus.
4)Then i open the generated .inp file in abaqus and apply material properties and submitted foe analysis.But still same problem is occURING.
Sir when i iam doing same procedure with clavicle as given in tutorials,it is working well in abaqus. I compare the both clavicle and femur .inp files which seems to same.
Sir one difference is only that when i export the femur bone from anybody i put the scaling factor 1 and prepare a stl file. When i open the stl in 3 matic i scale the file by 1000. Because mimics units are in mm. if i dont do it we are enable to prepare mesh. So question is that if i just open a stl file generated from mimics in anybody i scale down by .001 in anybody. But in case of mesh i dont play with scaling because we have to applied just loads by any2abaqus. Is it be the problem of the inconsistent units?
When i measure the lengh of mesh it is around 440mm. Is it possible that anybody assume the mesh lengh 440m.So there will be so difference between mesh length and actual bone lengh of the anybody model. Thats why loads are not uniformly distributed. Because we are also failed to visulize the loads in abaqus where clavicle bone loads are visualizing properly. Plz look into the matter.
Im attaching the all files generated.
Thanks.
Yes, your muscle attachments are in meters, whereas your mesh is in mm. Thus the misalignment problem occurs that i mentioned before.
RightFemur.inp:
*NODE
1, 84.3128, 1028.08, -162.976 <-------- mm
Output5.inp:
*node, nset=NS_MusclesSpineRight_PsoasMajor_PML4I_TM_1
100001,-0.023400,-0.070000,0.003700 <-------- m
Needs to be scaled. In the tutorial I specified a special transformation that could be used for the conversion purpose:
AnyFE2Abq.exe -i …\files_in\clavload.xml -o …\files_out\output.inp -m .\clavicula.inp r segment t “a11 a12 a13 a21 a22 a23 a31 a32 a33 dx dy dz”
If you set t to “1000 0 0 0 1000 0 0 0 1000 0 0 0” it should convert the muscle attachments to the right values.
Dear sir
i have done as you said. But error is still same. Plz check the transformation which i have done is in proper way or not.
AnyBodyStudy Study = {
AnyFolder &Model = .Model;
***ERROR: THE DISTRIBUTING COUPLING WEIGHTS FOR COUPLING NODES LOCATED ON
SURFACE ASSEMBLY_ANYBODYSURFACE SUM TO 0.0000. THIS VALUE IS TOO
SMALL FOR PROPER BEHAVIOR OF THE ELEMENT.
This error is related to the next warning:
***WARNING: THE INFLUENCE RADIUS IS SMALLER THAN THE CLOSEST COUPLING NODE ON
THE SURFACE FOR COUPLING DEFINITION
You may need to add quotation marks to the string for the transformation to have an effect:
//include the next line to have a camera in the model
//#include "Model/MovingCamera.any"
}; // End of study
// Include an operation sequence to run all required steps of your application (see Operations tab) #include “<ANYBODY_PATH_TOOLBOX>\Operations\RunAppSequence.any”
Sir
Its works model loaded but in abaqus problem is still same. Loads and couplings are still can not vizulize. And still error are same. Now i thinks units are consistent.
*node, nset=NS_MusclesSpineRight_PsoasMajor_PML4I_TM_1
100001,-0.002340,-7.000000,3.700000
*coupling, constraint name=CON_MusclesSpineRight_PsoasMajor_PML4I_TM_1, ref node=NS_MusclesSpineRight_PsoasMajor_PML4I_TM_1, surface=anybodysurface, influence radius=638.711717
*distributing, weighting method=UNIFORM
*node, nset=NS_MusclesSpineRight_PsoasMajor_PML4I_TM_2
100002,-0.002340,-7.000000,3.700000
etc.
Why this error is still coming.
Coding are
FileName =“Output\AnyFE2Abq\AnyFE2Abq.exe”;
Arguments = “-i .\Output\rthighload.xml -o .\Output\Output6.inp -m .\Output\rightfemur.inp -rsegment -t” +strquote(".1000 0 0 0 100 0 0 0 1000 0 0 0");
WorkDir=".\ ";
Thanks.
};
it works,file is loading genarated files are attached and how mesh is looking are also attached. Some contraints dispalying but abaqus is still giving same errors on analysis.
Thanks.
the problem is that your output and your mesh are not aligned. You can see it from your screenshot. The muscle attachment nodes are not anywhere close to the bone surface - means you have used the output ref. frame that is not related to your mesh at all, thus the problem.
Please align them. As I have mentioned before - try adding the drawing of the STL surface into the ref. frame used for outputting the muscle forces - it should lie on top the AnyBody surface (please bear in mind that your mesh is in mm). That’s the ultimate test. If the AnyBody bone and your mesh are not on top of each other - you will not get things to work.
Secondly, you can look at the value of the influence radius - 639mm means that your muscle attachment are almost a meter away from the bone. They should be 0-10mm or something like that.
If you still do not have an idea how to align your FE and AnyBody bones - please read all tutorials on the FE interface. The ANSYS section explains it partially.
Thanks sir
One question is that i exported anybody standing man right femur bone. I prepared the mesh of that bone. So why we need to align the mesh with anybody bone. Because it is of the same size and shape.
