Problem with GAP element

[nia21209]

Hello Calculix comunity,

I have a problem with the GAP element. To test the GAP element I have created a simple C3D8 element with a displacement boundary condition (compressive stress) applied in the x-direction at four nodes. The element is stretched in the transverse directions by the compression. I then defined a node (*NODE 101) with a gap in the z-direction of 0.03 mm and connected it to the underlying node of the C3D8 element in the GAP element card. As soon as the C3D8 element is now stretched more than 0.03 mm transversely in the z-direction the GAP is closed. To better understand the model, here is the .inp file:

*node, nset=Nall
1, 0.0, 0.0, 1.0
2, 0.0, 0.0, 0.0
3, 0.0, 1.0, 1.0
4, 0.0, 1.0, 0.0
5, 1.0, 0.0, 1.0
6, 1.0, 0.0, 0.0
7, 1.0, 1.0, 1.0
8, 1.0, 1.0, 0.0
** -----------------------------------------------------------
*element, elset=C3D8,type=C3D8
19, 1, 2, 4, 3, 5, 6, 8, 7,
** -----------------------------------------------------------
*nset, nset=fix_y
2, 1, 5, 6,
*nset, nset=fix_x
3, 2, 1, 4,
*nset, nset=fix_z
2, 4, 6, 8,
*nset, nset=pres
5, 6, 7, 8,
** ------------------------------------------------------------
*MATERIAL,NAME=az31b
*ELASTIC
41067.,0.3

*SOLID SECTION,MATERIAL=az31b,ELSET=C3D8
** -----------------------------------------------------------
*NODE
101,1.,1.,1.03

*ELEMENT, TYPE=GAPUNI, ELSET=Egap0
20, 101, 7
*GAP,ELSET=Egap0
0.03,0.0,0.0,-1.0,1e12,1e-3

*BOUNDARY
101,1,3,0.

** -----------------------------------------------------------
*TIME POINTS,NAME=T1,GENERATE
0,1,0.1

*AMPLITUDE,NAME=A1
0,0.,
1,1

** -----------------------------------------------------------
*STEP,NLGEOM,inc=1000000
*STATIC
0.1,1,1e-6,0.1

*BOUNDARY
fix_x,1,1,0.
fix_y,2,2,0.
fix_z,3,3,0.

*BOUNDARY, AMPLITUDE=A1
pres,1,1,-0.15

*EL PRINT,ELSET=C3D8,TIME POINTS=T1
S,E

*NODE FILE,TIME POINTS=T1
U,RF

*EL FILE,TIME POINTS=T1
S,E,SDV

*END STEP
** -----------------------------------------------------------
The closing of the contact works, which is why the node at (1,1,1) has only a maximum displacement D3=0.03.

What now irritates me very much is that when the contact is not yet closed (Time 0.5), a different stress SXX occurs at the node (1,1,1) than at the nodes (1,0,0), (1,0,1) and (1,1,0).

The GAP element should not introduce any force yet and in any case not in the x-direction. Do I have a problem here or is this possibly a software error?

I would be very pleased about your help.

Best Regards
Anton Nischler

[vicmw]

Is your *GAP data line as intended? It looks like:
1e12 not used
1e-3 spring stiffness

[nia21209]

Hello Victor,

Thank you for your reply. You are right. The line actually reads:

*GAP,ELSET=Egap0
0.03,0.0,0.0,-1.0,1.e12,1.e-3

However, this has no influence. In general, there should be no influence in the x-direction from the GAP element, or? Especially if the GAP is not yet closed.

Looking at the nodal forces F1, where the displacement is initiated, all of the four nodes have the same value as expected (Fig.1). Only the stresses SXX are different.

It is also very strange that the stress SXX at the node with the GAP element is exactly half of the expected stress (at the 7 other nodes).

When I run the FEM simulation without the gap element, the correct field quantities are obtained (Fig. 2).

I’m not sure, but is it possible that the GAP element has an error?

Best Regards
Anton

[Disla]

@nia21209

very strange that the stress SXX at the node with the GAP element is exactly half of the expected stress (at the 7 other nodes)

Are the displacements as expected?.

¿Is it possible that what you see is the node average value between the solid part SXX and the GAP Element Side SXX=0?

[nia21209]

Hello Disla,

thank you very much for your great help! It’s exactly the Problem! I’ve checkt the .dat file and at the integration points the stresses are correct.

Any suggestions on how to get cgx to not output the average stress?

[xyont]

to eliminate averaging due to extrapolated from integration point, generally constraint need to be use

in this case, may the model approach use duplicated nodes and connect them with equation will work.

[xyont]

@nia21209

Any suggestions on how to get cgx to not output the average stress?

[nia21209]

Thank you very much xyont!

[Disla]

¿Do you think it would be possible to avoid average on shell elements?

[xyont]

general constraint using equation is low level method, it seems can be used in many cases including connected of shell element nodes.

noticed, it’s required to use with caution since improperly definition or unbalanced in ratio may lead to violating equilibrium.

[JuanP74]

use *TIE to connect disjointed meshes so the .frd file data is not averaged. You can do that instead of using coincident nodes to have non averaged results in different regions of the same solid or solid/shell combination. So far it has worked pretty well for me.