hi, I am working on welding joints using mechanical workbench. in my model the initial contact information show a maximum geometric penetration and geometric gap of amount 5.8878e-017m compared to a pinball radius of amount 1.3539e-004m. I wonder if these values are normal and acceptable. if not, how can I delete the geometric gap and penetration?
The values you mentioned are parameters for defining contacts and define how contact should perform in the analysis. For example, in a thermal analysis if you define a pin ball radius, then heat will be transferred only through those nodes that are located within the pin ball area. Therefore, these numbers are application base and can be different. You can disable the Pin ball effect, however gap distance should always be defined. Regarding penetration, if you are using Steady-State Thermal module you don't have this parameter in contact at all. I think you want to use static structural analysis and perform a Multiphysics simulation, then it is possible to have this parameter since you are performing a structural-thermal analysis. These are my assumptions since you have haven’t explained what module you used. Hope this information helps.
Dear Mr. Ahmadi
I am using static structure and the applied load is bending fatigue.
Dear Ahmed,
Basically even though in CAD geometry we consider two surfaces in perfect contact it is not the case. There are small penetrations or gaps in the surfaces since CAD geometry since these surfaces are mathematical approximated.
So these tolerances have to be accounted in simulation software.
In contact detection ANSYS calculate distances between nodes/guass points in surfaces to see if the contact surfaces are open or closed.
" The pinball region is involved with the distance from contact element to target element in a given contact region. Outside the pinball region, ANSYS doesn’t bother to check to see if the elements on opposite sides of the contact region are touching or not. The program assumes they are far away from each other and doesn’t worry about any additional calculations for the most part."-http://www.padtinc.com/blog/the-focus/be-a-pinball-wizard-with-contact-regions-in-ansys-mechanical
Considering the values you have reported for pinball radius and geometrical gap it seems that these values are automatically generated by ANSYS. I think these values(geometrical gap/penetration) are just geometrical tolerance between the surfaces, and I suppose the initial contact is in "closed" status.
If you even wish the solver to neglect these tolerances you can use "adjust to touch" option in "Geometrical modification> Interface treatment" setting in the particular contact option. But be aware that this will adjust every node/element(in pinball region) in the contact region to be in closed contact.
For more info please refer.
-https://www.sharcnet.ca/Software/Ansys/17.0/en-/help/wb_sim/ds_geometric_correction.html
-http://innomet.ttu.ee/martin/MER0070/WB/WS9/Connections/Mechanical_Intro_15.0_L06_Connections.pdf
Dear Mr. Rashiga
Thank you for your nice reply, unfortunately, the interface treatment option is not available for bonded contact which is the kind that I am using in my model. So, I wonder if there is any alternative.
Regards
Dear Mr. Ahmed,
My opinion is if the surfaces are in bonded contact and if the initial contact status is closed, you do not need to worry about the gap/penetration.
Also I don't think you will be able to remove that penetration/gap.
Best Regards.
Dear Ahmed,
If you use “Adjust to touch” option you don’t need to worry about anything (you can have a bit gap in your contact) and ansys will adjust the contact automatically, otherwise the state of the contact will be different in the middle of the analysis which may cause issue. Hope that helps. By the way, in your question you mentioned welding joint, therefore, I thought you may wanted to simulate welding effects. For that reason I explained a bit about structural-thermal analysis.