Your question is a bit ambiguous. What do you mean by "to derive" exactly.

@Hamidreza, thanks for your concern and my apologies for the ambiguity.

What I mean is to calculate the nodal contact pressures by using the contact forces of CONTA178 elements and the geometric information of the underlying elements of CONTA178 elements, or possibly some other necessary information.

Thank you again.

Hello Cao,

I don't have previous knowledge in ANSYS, but something I use to do when I need to determine the contact pressure distribution from nodal contact force values, is to assign an equivalent area to each node, and then divide the contact force associated with this node by its equivalent area.

For example, in a triangular mesh, the equivalent area of a node would be 1/3 of the area of each element attained to it.

It may not be the best way to determine the contact pressures, but I could give a good approximation. 

Hope that helps!

Regards

If somehow you are limited to use only CONTA178, the method that Victor described gives you a good estimation of how much would be the pressure, however if you model this problem in ANSYS Workbench, you can insert a Contact Tool in your Solution and then you will be able to insert different type of contact relate result such as nodal pressure, nodal force and etc. Even by inserting User Defined Result, you will be able to do the same and extract the contact related result from contact nodes.

@Hamidreza, thank you for your kind advice.

Actually, for the time being, I am more familiar with classic ANSYS Mechanical and APDL commands. I'd try ANSYS Workbench in the future. 

All the best.

@Víctor, thanks for your inspiring suggestion.

I've just tried your approach. For the contact bodies are meshed with PLANE182 elements (2-D 4-node), so the equivalent area of a certain contact node is 1/4 the summation of the areas of all PLANE182 elements attached to it. Then the contact force of this node is divided by the equivalent area. But what a pity, the resulting contact pressure is not consistent with the analytical value (K. L. Johnson, Contact Mechanics, Cambridge University Press, 1985), and the results changed when I refined the mesh.

I've also tried using the APDL get function ARNODE(N) to calculate the equivalent area. But also failed.

Finally, I use the following steps to calculate the contact pressure of a certain contact node "n" (please see the schematic drawing in the attachment).

1. An intermediate "element pressure" Pn-1 is calculated by dividing the average of the two contact forces Fn-1 and Fn by an equivalent area Ln-1*t, where Ln-1 is the boundary edge length of element En-1, and t is the element thickness (usually 1), i.e., Pn-1 = (Fn-1/2 + Fn/2)/(Ln-1*t). In a similar way, another "element pressure" Pn = (Fn/2 + Fn+1/2)/(Ln*t).

2. The corresponding contact pressure Rn = (Pn-1 + Pn)/2.

The results show good consistency, with coarse or finer mesh, with the analytical ones and the ones obtained using surface-to-surface CONTA171 elements!

All the best.

Dear @Cao and @Hamidreza, thanks for sharing your knwoledge.

Hello Cao,

Use ASEL command to select your area(s) and after SFA,ALL,1,PRES,Value. Where Value=Force/Area. After finishing with all of your areas use ASEL,ALL to keep in memory the entire set of areas for display purposes.

Good information Cao NIU.

valuable information Cao