Learning Forum

[hesamkeshavarzz]

Hi everyone.

I wanna export residual caused by bending to another static structural analysis in such a way that I have no strain in the second analysis. but as soon as I import the stress, the solution button get active and leads to strain. briefly how can I export residual stress without making strain in the second static structural?

Thanks 

 

[peteroznewman]

Is your goal to combine the stress from the first analysis with the stress from a second analysis?  If so, what you describe is not how you do that. Instead, you create a project with both analyses in it and use the Solution Combination feature to add the stresses together in a new result.

https://innovationspace.ansys.com/forum/ansys-bing-search/?q=solution%20combination

[hesamkeshavarzz]

Thank you so much dear Peteroznewman for your quick reply. let me paraphrase, Imagine that you have a bent shaft that is straightened and now you want to monut a diak by shrink fit on it. to do so you need to first bend the shaft and obtain residual stress, then you should apply this stress on a straight shaft in the second analysis. ok? I dont wanna compound two stresses, If I wanted to do so the job was so straightforward and could be done in 2 load steps. In fact I want to model shrink fit in a shaft cut from a prestressed metal 

Thanks a million 

[hesamkeshavarzz]

Hi

dear @Peteroznewman I would be so grateful if you could help me

Imagine that you have a bent shaft that is straightened and now you want to monut a diak by shrink fit on it. to do so you need to first bend the shaft and obtain residual stress, then you should apply this stress on a straight shaft in the second analysis. ok? I dont wanna compound two stresses, If I wanted to do so the job was so straightforward and could be done in 2 load steps. In fact I want to model shrink fit in a shaft cut from a prestressed metal.therefore I need to export my undeformed shaft that has no strain meanwhile carry residual stress with it. but When I map my residual stress to the second analysis the solve button gets active.

any help will be appreciated.

[peteroznewman]

Use a multistep model with step dependent contact control and step dependent loads and supports. The shaft and disk with a hole are in the model.  The shaft must have a plasticity material model.

Step 1.  Frictional contact between shaft and hole are turned off. A constraint supports the disk. A temperature load causes the disk and hole to expand.  A force is applied to bend the shaft.

Step 2. The bending force reverses to straighten the shaft.

Step 3. The force is ramped to zero.

Step 4. Frictional contact between the disk and shaft becomes active.

Step 5. Temperature load on disk returns to room temperature, disk shrink fits to shaft.

Step 6. Support for disk is disabled.