Cancel
Showing results for
Did you mean:

# SOL 101 Contact Inaccurate results?

Pioneer

Hi,

Trying to learn contact analysis using Femap SOL 101 solver and thus picked up some standardized test cases.

This particular problem involves performing a linear contact analysis between solid & shell elements.

The set up is shown below:

Contains solid elements blocks, the base which is fixed in all directions. The plate is suspended 0.05" above the solid block upper faces. The plate has a pressure load applied downwards so that they make contact with solid blocks. Certain nodes in the plate are constrained in X & Y directions to prevent rigid body motion. The blocks are of "Softer Materials" and plate is Aluminum 2024-T3.

Model Setup

The contact card is shown below. I've played with different settings. Plugging in a small value for friction (0.05 to 0.1), varying Max search distance (0.055 to 0.1), running with include shell & not include shell thickness options, setting initial gap/penetration to 0 etc.

Contact Property Card Definition

Have created 3 contact regions. Left Solid upper face, right solid upper face and shell. I've made sure that shell elements bottom elements are the ones in contact.

But when I run the analysis, I get the following deformation pattern:

There is some penetration of the solid by the shell.

Deformation Pattern

And finally an output vector called Contact Pressures is presented. So if I want to find out total stresses for the elements circled in the image below, then do I need to add contact stress values to an additional output vector like Von Mises? Or does Von Mises output vector already factor in stresses due to contact?

Contact Pressure OutputShell Von Mises Output

Would appreciate some insights.

Thx

7 REPLIES

# Re: SOL 101 Contact Inaccurate results?

Legend

I guess that the penetration you are seeing is due the scale you used for the plot. put scale deformation 1 and check contact gap/penetartion to check the real value. If the penetarion is large you can play with the autopenalty or penalty factor. check if the resulrs change a lot.

About stresses you do not have to add pressure to Von Mises.

Anyway looking the model I guess you will have singularity due to edge contact to read stresses there

# Re: SOL 101 Contact Inaccurate results?

Solution Partner Phenom

Dear FN2000,

Here you are a few suggestions:

• In contact "no penetration" problems the use of symmetry BCs is critical, this is the best natural way to "stabilize" your FE model, do not constrain randomly nodes, in your case you can study 1/4 model because you have symmetry in both loads & geometry, simply prescribe symmetry BCs in all nodes of plane YZ (ie, TX=RY=RZ=0) and plane XZ (ie, TY=RX=RZ=0) and you are done!!.
• Second, this is a LINEAR CONTACT problem where displacements are small, then use scale factor 1:1 for deformation, because FEMAP shows the trending deformation using a big scale factor. Click in ACTUAL DEFORMATION and next use SCALE DEFORMATION 1.0, this way the "apparent" penetration will disappear, OK?.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

# Re: SOL 101 Contact Inaccurate results?

Pioneer

Thanks folks.

I never really thought about deformation scale or resolution. A small but important detail, eh? Duh!

Jon_Morga, if I understood your reply correctly, it seems like Von Mises output contains contact pressure as well? If yes, then what is the use of contact pressure output?

The last question may seem obvious but I would like to know.

# Re: SOL 101 Contact Inaccurate results?

Legend

I will try to explain it

The contact pressure is the value in the direction of the normal establishes between surfaces. Von mises is calculated from stress tensor caused by this pressure.They are two different things.

I hope the explanation is enough

# Re: SOL 101 Contact Inaccurate results?

Pioneer

Thanks for clarification Sir

# Re: SOL 101 Contact Inaccurate results?

Phenom
Couple of other things to keep in mind...
1. The contact solution prevents the Source Region nodes from passing through the Master (target) region segments. So the position and refinement of the Source region nodes compared to the Master target element faces influences what can or cannot pass through or rotate over the edge of a pair of contact interfaces.
2.Plate elements only address 2D stress... bending, membrane, shear. None of the calculated stresses are "Z direction", other than the variation of bending stress based on fibre distance. Contact stress is a surface normal stress based on the contact forces and element area. The plate Von Mises stress will be "related to" the contact stress, but mostly independent. 3D elements calculate Von Mises stress using the 3D stress state. Plate Von Mises stress only uses the in-plane stresses and the Z stress is non-existent/ignored.

# Re: SOL 101 Contact Inaccurate results?

Pioneer

Regarding Point #2, what does it mean for Post-processing? Do I have to use an interaction equation to factor the presence of both in plane & normal stress vectors?

What are the best practices regarding the above?