Hi all, I am running ABAQUS/Explicit incremental metal forming simulation. The tool radius=3mm, blank mesh=0.5mm, blank thickness 0.8mm, shell S4 element, friction=0 now. tool speed up 20 times faster than experiment, with mass scaling to target 5E-6. time scaling factor=0.7. damping alpha=10.
However, the simulation stops automatically with the following error:
Excessive incremental rotation of the elements in element set ErrElemExcessIncrementalRotation-Step1.
There is only one element with excessive rotations
Anyone has ideas? Thanks!
Dear Zhong Chen, it would help if you could provide a screenshot of your model or the calculation result (if this is available).
Hi Rudiger, Thanks for your attention.
1. I 've attach a picture.
2. I checked .sta file, it shows warning:
***WARNING: For contact surface ASSEMBLY_SHEET-BOT-SURF, some facets are
thicker than 0.6 times an edge or diagonal length of the facet
(for example, the thickness is 1.60000 times the element size
for the facet on parent element SHEET-1.2701). This may lead to
unstable contact involving the bull-nose extension on the surface
perimeter, which could be avoided by using the MAXRATIO parameter
on *SURFACE.
Thus, I am using MAXRATIO=0.9 now and wait to see the results.
Any ideas?
You can try applying velocity/rotation boundary condition to the part at initial. This may work for you.
Hi Mr. Cheng
I have a similar problem. I am carrying out a simulation of deep drawing model using ABAQUS. I would like to know if you were able to solve your problem. And if so how.
Saludos, yo tenia el mismo error, y se debía a que no habia colocado suficiente tiempo en los steps.
Dear all
I think you can try reducing thedimension of the minimum time increment.
Probably the problem is the mass scaling factor.
I agree with Francesco.
Try not to set any value to the time scaling factor, just select a little bit lower stable time increment (maybe 1E-6 could be good).
Keep us updated.
Regards,
Antonio
can anyone help me to rectify the following error:
For a self contact surface, the facets of the elements in element set ErrElemFacetThick3d-Step1 are thicker than the edge or diagonal lengths of the facets. Use the MAXRATIO parameter on *SURFACE to allow automatic rescaling of the contact thicknesses where necessary for this surface. Refer to the status file for further details. where can i find * surface and MAXRATIO ?
Abir Abdelkefi Were you able to find how to input *MAXRATIO ? I saw in the documentation that this can be edited through input (.inp) file.
Cheers.
I just come to know now. Thanks a lot for the information, do you have any idea about which kind of interaction should be choosen for the incremental forming process, i'm trying with surface to surface and penalty contact. however i have remarqued a delay in the deformation (after 3 of 4 cycles, i show a deformation but not in the begining which could be explained by the choice of interaction or mechanical constraint formulation )@ Achuth Sreenivas
Abir Abdelkefi I do not understand by 'delay in deformation'. If you have surfaces with complex shapes in contact for the explicit step, it is better to use surface-to-surface interaction with penalty constraint formulation. However, this may cause large values of penetration depending upon the model complexity. Otherwise you can use Kinematic constraint which is strict with contact penetrations. This may lead to severe distortions in elements.
Hope this helps.
Achuth Sreenivas 'delay in deformation' that means that the deformation starts later after few cycles. I have already used surface-to-surface with penalty constraint however i find the same problem, moreover i don't have any friction between the tool and the sheet. I'm trying before with implicit analysis by using node to surface and it works but now with explicit i do know where is the problem in contact.
Abir Abdelkefi I cannot be sure about what the problem is until I can see your model. But there could be few possibilities:
- May be the problem with penalty constraint. Try using Kinematic contact method in contact formulation .
- It may not be the problem with contact formulation if it had worked with implicit. There may be some dynamic effects. Check Kinetic energy to internal energy ratio percentage value. It should be below 5%.
- For explicit step, you would have defined amplitude for tool movement because it is required. For implicit this is not required. Check the amplitude values if you have not done this before.
Cheers.
Nizar El-Achab
Some tips for incremental forming via Explicit:
1. increase tool speed. but not too fast for dynamic oscillation. check energy ratio.
2. mass scaling, either automatic or fixed. or target dt=5E-6, for example. but not too large for dynamic oscillation.check energy ratio.
3. control output #
4. use symmetry for model if possible
5. use rigid tool
6. integration point # through sheet thickness. try 3, 7, 9, etc. fewer is faster.
7. time scaling factor, try 0.5,0.7, 0.9 etc.
8. mesh size. not too small for stability limit reason. not too large for accuracy issues.
9. friction. larger value needs more computation time.
10. single precision is about 20% faster than double precision. but double is usually preferred for accuracy.
Good luck.
-Zhong
Zhong Chen
Hi Zhong Chen, I have the same error "Excessive incremental rotation of the elements " when I run my incremental sheet forming simulations with shell elements (S4R) on ABAQUS. I tried to refine the mesh but the same error. When I used 3D elements, I have never had this issue. Could you please let me know if you have solved this problem and how? Thank you very much.
- Badges
- Science topic