## General Mechanical

#### Understanding variation in results using different contacts

• Saurabh
Subscriber
I have a model with all parts at maximum material condition (MMC). The parts have interference fit in its assembled state. I am trying to simulate the stress distributions for the components at assembled state at MMC. What is the correct way to perform the analysis? Please help.

1). I did the static structural analysis using frictional contacts using "Adujust to touch" since there is already geometric penetration as shown by initial contacts generated. I get the equivalent stress values which are very low.

2). I did the static structural analysis using frictional contacts using "Added offset, add ramped effect" thinking that will seperate the physical boundaries which is more close to practical. I get the equivalent stress values as very high.

In both cases I am using the same number of elements, meshing, frictional coefficient and boundary conditions.

Please see results below:

Can somebody help me undersatnd which is the correct method to model this and why.
Thank you.
• peteroznewman
Subscriber

Dear Saurabh,

Adjust to Touch zeros out the geometric interference that was present in the geometry which is why you got very low stress results.

Added offset, ramped effects (assuming you use the default value of 0), correctly resolves the geometric interference. The stress you see is the result of the interference. If the mesh on both sides of the frictional contact has node-to-node alignment, that is the best situation. If the mesh is coarse and you have linear elements, then you can get artificially high stresses due to a node on one side being inside the straight line edge of the other side. Using quadratic elements will allow the element edges to follow to curve of the geometry.

• Saurabh
Subscriber
Hello Peter,

Thanks a lot for your response. This explanation helps me understand the concept better. I will check the meshing as you suggested. Appreciate your help.
• bhagwantP
Ansys Employee

Thanks Peter.

@Saurabh,

some more add on information for your reference from our help section:

Geometric Modification (ansys.com)

Thanks

Viewing 3 reply threads
• You must be logged in to reply to this topic.