Questions regarding the modeling of a press fit 2

[ProtoformX]

Hi. After getting used to the Ansys language a little bit, I've come to prefer writing input files rather than using the interactive GUI. With that being said, I have some questions about how to model the contact pairs for a 2-D axisymmetric press fit of a flywheel on a shaft using /prep7 command lines, basically how can I do the same thing that the contact wizard does? I know that contact and target elements must be meshed along the lines defining the press fit interface, so do I just use the LMESH command? Do I have to define any advanced options like outward normal direction, and if so how?


Another question pertains to press fits in general. If I have 2 different materials for my flywheel/shaft assembly of equal axial length, should the contact pressure be minimum or maximum at the axial ends? For most of my analyses using the contact wizard, I'm getting a maximum near the ends, and I'm also getting a warning that there may be too much initial penetration for a few contact elements. Are these possibly related?


Thanks in advance.

 

[Drej]

> how can I do the same thing that the contact wizard does?

Remember that every action you do in the GUI is just converted internally into the appropriate ANSYS command. After each action you do in the GUI go to List > Files > Log File. The log file is a list of equivalent GUI commands used. Just copy all of those commands to create your input deck, but be aware the log file lists EVERYTHING you do in the GUI including Zoom, Pan, etc.

> I know that contact and target elements must be meshed along the lines defining the press fit interface, so do I just use the LMESH command?

Yes if you want to. An easier way to create contact eleemnts is to use the ESURF command (which is how the contact wizard operates).

> Do I have to define any advanced options like outward normal direction, and if so how?

You can redefine the normal of a line (LREVERSE) or shell (ENORM) as you need to. In the contact wizard check the normals are pointing to one another and then reverse these if needed using LREVERSE.

> Another question pertains to press fits in general. If I have 2 different materials for my flywheel/shaft assembly of equal axial length, should the contact pressure be minimum or maximum at the axial ends? For most of my analyses using the contact wizard, I'm getting a maximum near the ends, and I'm also getting a warning that there may be too much initial penetration for a few contact elements. Are these possibly related?

Very difficult to know without seeing your model. Check visually to see your penetration using /post1 (you can contour this also). If you are not happy with the level of penetration (it's only a warning though) and you're using linear materials then try increasing the contact stiffness FKN by factors of 2 (it is a real constant and defaults to 1) until your model fails to converge and then recheck the penetration to see if there is any improvement.

Cheers,

-- drej --