Hi Louise,
it's ok then. Yeah, I remained that PBC as it is and just changed the voxel no. By the way, I got this message once I changed the voxel to 100 to all the axes.
Discrete field "TEXGENORIENTATIONVECTORS" is created for distribution "TEXGENORIENTATIONVECTORS".
WARNING in the keyword "*elastic", file="AnakIkan.inp", line=2096880: Errors in reading keyword data. rowid > numRows
WARNING: Unknown assembly level node set CONSTRAINTDRIVER0. This occurred while creating a load.
WARNING: Unknown assembly level node set CONSTRAINTDRIVER1. This occurred while creating a load.
WARNING: Unknown assembly level node set CONSTRAINTDRIVER3. This occurred while creating a load.
WARNING: The following keywords/parameters are not yet supported by the input file reader:
---------------------------------------------------------------------------------
*NSET, UNSORTED
The model "AnakIkan" has been imported from an input file.
Please scroll up to check for error and warning messages.
From the previous trial I don't have problem with the load creation. Are these warnings caused by the mesh generation as well(the one that I highlighted in red)?
TexGen 3.4.0 export to ABAQUS 6.10-1
Moderators: Martin, Developers
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Yanie,
I've no idea what is causing the errors highlighted I'm afraid. Have you checked the .inp file on the line where the first error was highlighted. Maybe this will give you a clue as to what the problem is.
Louise
I've no idea what is causing the errors highlighted I'm afraid. Have you checked the .inp file on the line where the first error was highlighted. Maybe this will give you a clue as to what the problem is.
Louise
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Dear Louise,
I've checked with the inp files related to this matter. I found out that the error is referring to the Equation section (PBC) and keep mentioning about "WARNING: Unknown assembly level node set CONSTRAINTDRIVER0. This occurred while creating a load." which are in the same section as well.
I totally have no idea why this thing happen because the PBC is automated generated in the exporting files right?
Hope you could give me some idea on this.
Yanie
I've checked with the inp files related to this matter. I found out that the error is referring to the Equation section (PBC) and keep mentioning about "WARNING: Unknown assembly level node set CONSTRAINTDRIVER0. This occurred while creating a load." which are in the same section as well.
I totally have no idea why this thing happen because the PBC is automated generated in the exporting files right?
Hope you could give me some idea on this.
Yanie
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Yanie,
I think you just found a bug! The node sets created are ConstraintsDriver0 etc. In all the Equations sections and Output Requests this is what is used but in the Load Cases section it is output as ConstraintDriver0 etc.
I have corrected this in the code but it won't go out until the next release (it will be in the code repository shortly). In the meantime if you go to the Load Cases section of your .inp file and change ConstraintDriver to ConstraintsDriver for all cases then, hopefully, it should work for you.
Louise
I think you just found a bug! The node sets created are ConstraintsDriver0 etc. In all the Equations sections and Output Requests this is what is used but in the Load Cases section it is output as ConstraintDriver0 etc.
I have corrected this in the code but it won't go out until the next release (it will be in the code repository shortly). In the meantime if you go to the Load Cases section of your .inp file and change ConstraintDriver to ConstraintsDriver for all cases then, hopefully, it should work for you.
Louise
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Louise,
It seems like doesn't work at all even I've changed the Load section. I still get the same warning which related to the boundary condition of the model.
WARNING in the keyword "*elastic", file="AnakIkan.inp", line=57304: Errors in reading keyword data. rowid > numRows (Below is the correspond line)
57304 *Equation
57305 3
57306 MasterNode8, 2, 1.0, MasterNode1, 2, -1.0, ConstraintsDriver1, 1, -28
57307 *Equation
57308 2
57309 MasterNode8, 3, 1.0, MasterNode1, 3, -1.0
Yanie
It seems like doesn't work at all even I've changed the Load section. I still get the same warning which related to the boundary condition of the model.
WARNING in the keyword "*elastic", file="AnakIkan.inp", line=57304: Errors in reading keyword data. rowid > numRows (Below is the correspond line)
57304 *Equation
57305 3
57306 MasterNode8, 2, 1.0, MasterNode1, 2, -1.0, ConstraintsDriver1, 1, -28
57307 *Equation
57308 2
57309 MasterNode8, 3, 1.0, MasterNode1, 3, -1.0
Yanie
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Yanie,
Do you get this warning when you run from the command line or just within CAE? If just within CAE then it may be a knock on effect from having problems reading the multiple node sets. The model still loads into CAE so that you can see the visualization of your model.
I can't see anything wrong with the .inp file so if you still have problems when you actually run from the command line get back to me and I'll ask someone in our group who's run the voxel mesh simulations using this output.
Louise
Do you get this warning when you run from the command line or just within CAE? If just within CAE then it may be a knock on effect from having problems reading the multiple node sets. The model still loads into CAE so that you can see the visualization of your model.
I can't see anything wrong with the .inp file so if you still have problems when you actually run from the command line get back to me and I'll ask someone in our group who's run the voxel mesh simulations using this output.
Louise
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Louise,
I get this warning when I run them in cae. I never try run my inp in command line since I found that the geometry is improper generated in cae. I keep trying changing the voxel no for every axes and it seems that I need to allocate more to it. I already tried up to 6 millions elements and it still failed. I think is must be the same generation between in cae and command line, right?
Is there any maximum values for the input of ABAQUS Voxel? I'm trying to run generate the geometry which is 56 nos of fibres in X direction and 28 nos fibres in Y directions. the height of the matrix is just 0.3 mm.
Yanie
I get this warning when I run them in cae. I never try run my inp in command line since I found that the geometry is improper generated in cae. I keep trying changing the voxel no for every axes and it seems that I need to allocate more to it. I already tried up to 6 millions elements and it still failed. I think is must be the same generation between in cae and command line, right?
Is there any maximum values for the input of ABAQUS Voxel? I'm trying to run generate the geometry which is 56 nos of fibres in X direction and 28 nos fibres in Y directions. the height of the matrix is just 0.3 mm.
Yanie
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Yanie,
Please could you try running from the command line and see if you still get an error? The problem is that, as there is a problem with loading into CAE because of the inability to match multiple node sets, we don't know if this then has an effect later in reading the file. If you try from the command line and still have the problem then we will know exactly what problem we are trying to address.
There shouldn't be a maximum value for the voxel export other than any possible memory issues if the number is too large. I think this would be a very large number as I rewrote the code to reduce memory usage.
Louise
Please could you try running from the command line and see if you still get an error? The problem is that, as there is a problem with loading into CAE because of the inability to match multiple node sets, we don't know if this then has an effect later in reading the file. If you try from the command line and still have the problem then we will know exactly what problem we are trying to address.
There shouldn't be a maximum value for the voxel export other than any possible memory issues if the number is too large. I think this would be a very large number as I rewrote the code to reduce memory usage.
Louise
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
HI Louise,
Sadly to say that the .inp still doesn't work even I ran it in command line. I guess the mistake is at the meshing level where I composed insufficient no of voxel. However, I've tried up to certain numbers of voxel and some parts it can't generate with regard to the input number. for instance, I put 2000 (X voxel), 1000 (Y Voxel), 5 (Z voxel) for a trial and it leads to unhandled exception error. That's the reason why I'm asking about the maximum amount of voxel to you previously.
yanie
Sadly to say that the .inp still doesn't work even I ran it in command line. I guess the mistake is at the meshing level where I composed insufficient no of voxel. However, I've tried up to certain numbers of voxel and some parts it can't generate with regard to the input number. for instance, I put 2000 (X voxel), 1000 (Y Voxel), 5 (Z voxel) for a trial and it leads to unhandled exception error. That's the reason why I'm asking about the maximum amount of voxel to you previously.
yanie
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Yanie,
I have been looking into this today. You may run into memory problems if you try to create 10 million voxels. I'm not sure what the upper limit is, however.
As far as the .inp file goes there is an error in the material definitions which is causing a problem. If you go to the materials section you will see, probably the first material which will be the matrix something looking like this:
*Material, Name=Mat0
*Elastic, type=ENGINEERING CONSTANTS
1e+009, 0.1
*Expansion
3e-006
This section should not have the "type=ENGINEERING CONSTANTS". If you remove this then it should work.
There also seems to be a problem with the Thermomechanical step at the end of the file which I'm still looking into. If you remove this final step then it works ok.
When you've run a job from the command line the .dat file produced will show you where the errors are in your input file.
Hope that helps,
Louise
I have been looking into this today. You may run into memory problems if you try to create 10 million voxels. I'm not sure what the upper limit is, however.
As far as the .inp file goes there is an error in the material definitions which is causing a problem. If you go to the materials section you will see, probably the first material which will be the matrix something looking like this:
*Material, Name=Mat0
*Elastic, type=ENGINEERING CONSTANTS
1e+009, 0.1
*Expansion
3e-006
This section should not have the "type=ENGINEERING CONSTANTS". If you remove this then it should work.
There also seems to be a problem with the Thermomechanical step at the end of the file which I'm still looking into. If you remove this final step then it works ok.
When you've run a job from the command line the .dat file produced will show you where the errors are in your input file.
Hope that helps,
Louise
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Louise,
Ok, I'll do the change and will update then. Thanks for your help.
Ok, I'll do the change and will update then. Thanks for your help.
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
HI Louise,
Forgot to mention before, do you think that I need to change my fibre sizes due to this Voxel matter?
YAnie
Forgot to mention before, do you think that I need to change my fibre sizes due to this Voxel matter?
YAnie
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Yanie,
Surely your fibre sizes are dictated by the textile you're trying to model?
Louise
Surely your fibre sizes are dictated by the textile you're trying to model?
Louise
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Dear Louise,
I ran the analysis with the recommended changes however it is still failed. I got 5 errors due to the changes in Material section and Thermomechanical step which concerning about hourglass stiffness and materials. Here I attached the 5 errors as mentioned earlier.
***ERROR: Problem when parsing keyword: ELASTIC
Invalid parameter: 3.5e+009. The parameter may be misspelled, obsolete, or invalid.
*** INPUT DATA IS READ FROM FILE MB0.ori
*Material, Name=Mat0
*Elastic,
***ERROR: UNKNOWN PARAMETER 3.5E+009
LINE IMAGE: 3.5e+009, 0.35
***ERROR: UNKNOWN PARAMETER 0.35
LINE IMAGE: 3.5e+009, 0.35
***NOTE: THE COMPLETED KEYWORD PARSED IS "*Elastic,3.5e+009, 0.35". PLEASE
CHECK IF THIS IS THE INTENDED USE OF THE CONTINUATION CHARACTER.
***WARNING: MPCS (EXTERNAL or INTERNAL, including those generated from rigid
body definitions), KINEMATIC COUPLINGS, AND/OR EQUATIONS WILL
ACTIVATE ADDITIONAL DEGREES OF FREEDOM
***ERROR: 771648 elements have been defined with zero hour glass stiffness.
You may use *hourglass stiffness or change the element type. The
elements have been identified in element set
ErrElemZeroHourGlassStiffness.
***ERROR: 771648 elements are missing elastic property reference. The elements
have been identified in element set ErrElemMissingElasticPropRef.
So, I make some changes on Elastic properties and i creates more errors then. I had adjusted the material section to cater the MissingElasticPropRef as below;
1st trial: *Elastic, type=ISO
3.5e+009, 0.35
*Expansion
6.5e-006
2nd trial: *Elastic,
3.5e+009, 0.35
*Expansion
6.5e-006
3rd trial: *Elastic, type=ISOTROPIC
3.5e+009, 0.35
*Expansion
6.5e-006
However, I got a lot of errors then correspond to this changes.
***ERROR: in keyword *ELEMENT, file "MB0.inp", line 1506181: Element number is not an integer for element of type C3D8R.
***ERROR: Node/element 153 cannot be found. Please check that it is defined.
***ERROR: Node/element 154 cannot be found. Please check that it is defined.
***ERROR: Node/element 155 cannot be found. Please check that it is defined.
Glad if you could contribute some ideas then.
Yanie
I ran the analysis with the recommended changes however it is still failed. I got 5 errors due to the changes in Material section and Thermomechanical step which concerning about hourglass stiffness and materials. Here I attached the 5 errors as mentioned earlier.
***ERROR: Problem when parsing keyword: ELASTIC
Invalid parameter: 3.5e+009. The parameter may be misspelled, obsolete, or invalid.
*** INPUT DATA IS READ FROM FILE MB0.ori
*Material, Name=Mat0
*Elastic,
***ERROR: UNKNOWN PARAMETER 3.5E+009
LINE IMAGE: 3.5e+009, 0.35
***ERROR: UNKNOWN PARAMETER 0.35
LINE IMAGE: 3.5e+009, 0.35
***NOTE: THE COMPLETED KEYWORD PARSED IS "*Elastic,3.5e+009, 0.35". PLEASE
CHECK IF THIS IS THE INTENDED USE OF THE CONTINUATION CHARACTER.
***WARNING: MPCS (EXTERNAL or INTERNAL, including those generated from rigid
body definitions), KINEMATIC COUPLINGS, AND/OR EQUATIONS WILL
ACTIVATE ADDITIONAL DEGREES OF FREEDOM
***ERROR: 771648 elements have been defined with zero hour glass stiffness.
You may use *hourglass stiffness or change the element type. The
elements have been identified in element set
ErrElemZeroHourGlassStiffness.
***ERROR: 771648 elements are missing elastic property reference. The elements
have been identified in element set ErrElemMissingElasticPropRef.
So, I make some changes on Elastic properties and i creates more errors then. I had adjusted the material section to cater the MissingElasticPropRef as below;
1st trial: *Elastic, type=ISO
3.5e+009, 0.35
*Expansion
6.5e-006
2nd trial: *Elastic,
3.5e+009, 0.35
*Expansion
6.5e-006
3rd trial: *Elastic, type=ISOTROPIC
3.5e+009, 0.35
*Expansion
6.5e-006
However, I got a lot of errors then correspond to this changes.
***ERROR: in keyword *ELEMENT, file "MB0.inp", line 1506181: Element number is not an integer for element of type C3D8R.
***ERROR: Node/element 153 cannot be found. Please check that it is defined.
***ERROR: Node/element 154 cannot be found. Please check that it is defined.
***ERROR: Node/element 155 cannot be found. Please check that it is defined.
Glad if you could contribute some ideas then.
Yanie
Re: TexGen 3.4.0 export to ABAQUS 6.10-1
Hi Yanie,
Abaqus is very particular about the syntax in .inp files.
You have left a comma after the *Elastic which means that it thinks that the following entry - 3.5E+009 is a parameter not the data. I don't know what is expected if you change it to ISO or ISOTROPIC. Please see the Abaqus User Manual to familiarise yourself with the expected parameters and data for the keywords.
Louise
Abaqus is very particular about the syntax in .inp files.
You have left a comma after the *Elastic which means that it thinks that the following entry - 3.5E+009 is a parameter not the data. I don't know what is expected if you change it to ISO or ISOTROPIC. Please see the Abaqus User Manual to familiarise yourself with the expected parameters and data for the keywords.
Louise