Hi Sir
i want to know that can i export loads on the surface mesh instead of volume mesh as a block diagram in abaqus interface tutorials suggested or Without use of any2abaqus?
2) I have a volume mesh of a femur with approx 800000 nodes. When im trying to exports loads using any2abaqus a zero kb output file is generating/ The size of mesh is 496mb. Is size and large no of nodes effects on the efficiency of any2abaqus?
Thanks.
Hi Mohit,
Yes, it does, it computes relative distances from the muscle insertion nodes to the mesh for the influence radius definition.
You can cheat a little bit - you can run the converter on the less dense mesh of the same bone and then simply replace the mesh file (it is included in the converted file). Replace the following line by your actual mesh.
*INCLUDE, INPUT=SURF_AVERAGE_LESS_DENSE.inp
You need to change the anybodysurfaceset definition too to account for the change in the element number - changes the following lines:
*elset, elset=anybodysurfaceset, generate
1,23969, 1
You will also need to change the indices of the newly created nodes to account for your large number. I believe the converter makes an offset of 200000 for the muscle insertion nodes.
*node, nset=NS_SomeMuscleHere
200001,-0.00213049,-0.001987,0.003353
for example to be:
*node, nset=NS_SomeMuscleHere
900001,-0.00213049,-0.001987,0.003353
(you can use “search and replace” in a text editor to do so or in some scripting languages).
Regards,
Pavel
Hi Sir
i apply the changes as you said at the top of text file of original mesh file and apply convertor. But there is still a zero kb output file is producing.
*INCLUDE, INPUT=SURF_AVERAGE_LESS_DENSE.inp
*NODE
*elset, elset=anybodysurfaceset, generate
1,23969, 1
1, 70.4985, -389.442, -1.42445
2, 52.7831, -390.627, -32.7181
3, 41.4673, -392.267, -42.3419
4, 60.5083, -390.521, -14.227
5, 63.835, -391.146, 1.58985
6, 40.083, -392.736, -40.3622
7, 56.6624, -391.559, -11.8696
8, 64.1042, -391.001, 0.573572
9, 63.1967, -391.39, 2.82503
10, 51.512, -394.242, 6.45581
11, 43.7877, -392.008, -39.4481
12, 69.2653, -389.731, -1.1422
13, 45.9894, -391.433, -40.5671
14, 47.5687, -391.011, -41.4762
so on.
Thanks.
I did not suggest to use them literally. I suggested to adapt to your case.
But if the XML file contains some loads and generated Abaqus code contains nothing - then there is some inconsistency again as we discussed many times. Units, for example.
Please do everything like in the tutorials.
Regards,
Pavel
Dear Sir
I have been resolved the above problem of large nodes. Now i export the loads on the femur with implant. Sir i want to share the work flow of the project to assure the steps-
- I export the anybody model femur with local reference frame with scaling factor1000.
- Then i export the femur in 3-matic. In 3-Matic i also design a hip impalnt, Then i cut the femur from oneside to assemble the femur and implant.Screenshot of assembly are attached. Then i apply materials on both and create a volume mesh.
- Then i apply loads by any body with that coding which you suggested earlier.
- Then i export the file in abaqus.
But when i run the analysis there are three errors that are displaying-
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. …for only 3 times
This error is same as i done the analysis of femur without implant earlier. Last time this error was for every node this time it si only for 3 times.
This error was due to the misalignment of reference frames.
My question is that -
1)Is my approach is right.or any chance of units mismatch. - How the implant scaling possible? Because tutorials only shows the scaling of source and target femur.
- How can i delete loads manually fron the genereated output. Because i thought if any load have large influnece radius so i want to delete this.
Thanks.
Hi Mohit,
The approach sounds OK to me. The devil is in the detail.
You get this error, because you exported the forces and called the converter for the full femur, am I right? This means there are about 3 forces with the influence radius that would touch the surface if it was the full surface. But since you have removed a part of the bone - it does not touch anymore and the problem occurs. You need to redefine this influence radius or remove the loads as you said. Alternatively you can select corresponding subsurfaces where these particular loads are supposed to be applied and connect it from the code manually. It will depend on the type of the operation you are modelling.
To modify something manually you can open the output file and remove the needed lines. I would strongly recommend to learn the keywords used in the output file before you delete or modify something. Please refer to the Abaqus Keyword Manual.
I believe from this point this is more of an Abaqus task rather than AnyBody.
Good luck.
Regards,
Pavel
Yes Sir,
You are absolutely right about the error. Sir i also planning to delete these lines
from the output files generated by the convertor. But i am enable to find exactly which are these loads or constraints are in text file? And also i want to know that if i edit a value in text file for eg.*node, nset=NS_Leg_Mus_GastrocnemiusMedialis1_5
100043,72.431838,-403.476220,47.204856
*coupling, constraint name=CON_Leg_Mus_GastrocnemiusMedialis1_5, ref node=NS_Leg_Mus_GastrocnemiusMedialis1_5, surface=anybodysurface, influence radius=15.229476
i just want to reduce influence radius to 1 and save text files.
Is this changes will create a desirable change or not? Because i tried it,it is not working well. Loads position is not changing by this. And if i delete this from text file than abaqus showing a error that someone nodes are missing.
Thanks.
Hi Mohit,
As I said in the previous message it is already mainly an Abaqus, not an AnyBody task. I would strongly recommend to learn the Abaqus input deck syntax (refer to Abaqus Keyword Manual) and analyze what is exactly going on in the code prior to modifications.
Moreover, I don’t think it is appropriate to delete something from the output, since it will change the equilibrium of forces. What you should probably do is to run the converter on the resected bone mesh excluding the implant, where all forces without exceptions will be applied to the bone surface via the tie constraints. The only force that needs to be applied to the implant is the hip joint reaction force. You will need to modify the constraint between the load application node and the geometry - it has to be replaced by another surface, which you can define on the implant head. You can simply select the entire contact surface of the head.
Please check the last few paragraphs of the Abaqus lesson:
And once again - please learn the keywords to understand what is done.
Kind regards,
Pavel
Hi Sir,
I was checking the fea interface tutorials regarding abaqus, in the last few paragraphs there is a discussion about the influence radius. In the case of the clavicle it is set be the outermost point.I want to know that what is the mean of it and for which cases it has to be set outermost point or not. Is in the my problem it set to be outermost point or not ?
Thanks.
1 Like
Mohit,
It should be described in the keyword manual of Abaqus in detail (check *coupling). But the idea is that for this coupling constraint you specify a node and a surface, where the influence radius defines how much of this surfaces is connected to the node. Basically imagine a sphere with the centre in the node of interest, it may cut either nothing (it is when you get an error), a piece of the surface (the typical scenario for the converter), or contain the entire surface (influence radius defined by the outermost point max(r_i)). So in the example we made a separate surface representing the muscle attachment area and, thus, could simply use the “outermost point” option as it would take the entire surface automatically. This is exactly your case when you want to do the joint load - you need to select the surface of the stem head and make a constraint between this surface and the hip joint node.
Hope this helps.
Regards,
Pavel
Hi Sir
Thanks this trick is working well. One think which still remain problem to me related to material properties.I just want to know yours opinions about that-
- As our mesh is in mm so we scale our anybody model by the string(equal to mesh). So forces are also scaled. So im now confused that is i have to apply material properties according to GPA or MPA parameters?
- if the material properties are applied to meshes(individually to implant and bone) before any2abaqus convertor ,then if i apply convertor ,then in outputfile which i have to open in abaqus,retain these properties or not? This question i asking just for the following reason which i have seen in tutorials-
This reader is not fully compatible with the INP keyword language for Abaqus. Basically, it only reads in the first block of nodes (*NODE section) and it does not accept commands that may interfere with the interpretation of this node section. This implies that many Abaqus keywords are not allowed in front of the first node section.
Thanks.
Mohit,
I do not think you need to do anything if you scaled everything to be in mm. You should use your original units, but please bear in mind that the moment conversion (or the force conversion) - please check are not transferred correct while scaling the model (we addressed this one before). So this one has to be fixed if the problem is still there, but otherwise the converter will use the original mesh file and all the content without modifying it and will include in the beginning of the output file.
Regards,
Pavel
Hi Sir
I just create the assembly of implant and femur and apply desired material properties to both. And export the .inp file of the assembly and apply the convertor,i got output and i find that all loads and constraints are misaligned.Influence radius are becomming large.Even without doing this earlier when i dont apply material properties to parts everthing was working well.Why this is happening because femur and implant are same which i used earlier:confused:
Thanks.
Mohit,
I must send you to our previous discussions on the consistency of input. If something went wrong - you should compare your two cases and figure out. At this point we probably discussed all possible problems.
I could only recommend to take the successful case and keep working on that one.
Regards,
Pavel
Yes sir
Thanks for yours valuable support. I compare the both cases and probably i found the difference which i want to share with you. When everything was working well, then i considered implant and femur one part, i take both stl parts make assembly and prepare mesh in 3 matic.
In second case i take both parts individually and made the meshes of both separately. And then export both meshes to abaqus and apply material properties and done assembly. In the text file of first case it is showing one part and in the case of second it is showing two parts.
So in the first case everything working well but we are enable to apply material properties individually in abaqus because it is showing one part.
So we adopt second case but here i think that when we are applying scaling of anybody model by 1000 string,i think femur is becoming 1000 times large but implant remains same in that position,so that’s why this misalignment is occurring.
Thanks
Mohit,
the converter does not scale the mesh, but only the muscle locations coming from the AnyBody model (which is meters) and the magnitudes of forces and moments. Thus, your meshes should be consistent, unless they were originally created using different units.
Regards,
Pavel
Hi Sir
I think that convertor is not compatible with the material properties language. Because i resolve the previous issue but now i facing new problem. I apply materials to both. And run the convertor,loads and constraints seems to be ok in output file when i opened the output in abaqus but material properties which i assigned earlier is not showing in output. It showing a single properties without material.
Thanks.
I am not sure why it should not be compatible. If you have your mesh file with assigned material properties as: YourMesh.inp, the converter will use *INCLUDE keyword to include your previous file verbatim.
*INCLUDE, INPUT=YourMesh.inp
*elset, elset=anybodysurfaceset, generate
1,MAX_NODE_NUMBER_HERE, 1
*surface,name=anybodysurface,type=element
...
And I do not think there is anything wrong with the *INCLUDE keyword:
*INCLUDE: Reference an external file containing Abaqus input data.
This option is used to reference an external file containing a portion of the Abaqus input file.
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
Type: Model or history data
Level: Part, Part instance, Assembly, Model, Step
Abaqus/CAE: Several input data options in Abaqus/CAE provide the capability to reference external files;
for example, the material editor can read material properties from an ASCII file.
Reference:
• “Defining a model in Abaqus,” Section 1.3.1 of the Abaqus Analysis User’s Manual
Required parameter:
INPUT
Set this parameter equal to the name of the file containing the input data. See “Input syntax rules,”
Section 1.2.1 of the Abaqus Analysis User’s Manual, for the syntax of such file names.
Please check your meshes first and if you do not see the problem - try sending it to us.
Regards,
Pavel
Hi Sir
We are still working on the above problem in the hyper mesh software(implementation of material properties). Sir we have been implement your suggestion of in which we apply load on only femur part and then in abaqus doing assembly with implant mesh and edit constraints by surface of the implant. But in this we are getting the following errors during analysis-
THERE ARE 2 UNCONNECTED REGIONS IN THE MODEL SO INERTIA RELIEF ANALYSIS CANNOT BE PERFORMED.
What should i do now? Is i have to delete the inertia loads?
Thanks.
it probably means that you are missing some constraints, probably some nodes are floating in space. Please check.
Regards,
Pavel