A punch going into a material with fixed bottom

[Twaj]

I'm very new to abaqus and am currently working on a problem of a cylindrical punch compressing into an elastic/plastic material underneath it

I've made a cae which seems to start building but I constantly get the same problem of

ELEMENT TYPE C3D6 USES THE REDUCED INTEGRATION IN Abaqus/Explicit AND WILL BE REFERRED TO AS C3D6R FROM HERE ON

ELEMENT TYPE C3D6 USES THE REDUCED INTEGRATION IN Abaqus/Explicit AND WILL BE REFERRED TO AS C3D6R FROM HERE ON

There are 2 warning messages in the data (.dat) file. Please check the data file for possible errors in the input file.

The slave surface nodes in node set WarnNodeMassRatio3fix-Step1 have much larger masses than the nodes on the master surface. Significant contact noise may result. Suggested workarounds include setting the WEIGHT parameter so that what was the master surface becomes a pure slave surface in the contact pair, using mass-scaling to adjust the ratio of nodal masses, or using the penalty contact algorithm. See the status file for further details.

I was wondering whether anyone had any advise on the matter or a similar cad program which I can work from?

Thank you very much for you time

 

[corus]

The model is axisymmetric. Use 2D axisymmetric elements and then you'll avoid using wedge type elements altogether.

 

[Twaj]

Thank you for your input. I tried this, which actually did result in the program making some progress, however it is able to only compute the first four frames before becoming stuck.

I have these two errors

1. Boundary conditions are defined at the nodes contained in node set WarnNodeBcIntersectKinCon. In addition the nodes are also part of a surface involved in kinematic contact. The kinematic contact constraint will be overridden by the boundary conditions in case of a conflict. Penalty contact may be used instead.

2. The slave surface nodes in node set WarnNodeMassRatio3fix-Step1 have much larger masses than the nodes on the master surface. Significant contact noise may result. Suggested workarounds include setting the WEIGHT parameter so that what was the master surface becomes a pure slave surface in the contact pair, using mass-scaling to adjust the ratio of nodal masses, or using the penalty contact algorithm. See the status file for further details.

I have a boundary condition at the bottom of the material, holding it in place, and the other is one holding the centre axis of the punch in place

I can't for the life of me figure out what the second error is telling me however.

Thank you for your time

http://files.engineering.com/getfil...b-383f-4e1d-b661-402c10cc8e8a&file=Axisym.cae

 

[corus]

Don't use reduced integration with contact, you get severe hourglassing with those elements. Just untick the reduced integration box on the element type. In addition, refine your mesh, particularly with the lower block. The mismatch in element size will cause problems. The model would be better if you partitioned the lower block where the upper block meets it, and then mesh it. The 2 meshes will line up then if you have the same seeding. I also removed the boundary condition on the line R=0. For a solid cylinder there's no need to apply a symmetry boundary condition on the axis as this is implied with the geometry. That'll remove any warnings about boundary conditions and contact surfaces etc. Lastly, why is this a dynamic explicit analysis? I ran it up to about 12 seconds with a static general analysis when it failed with too small a time increment. Probably a much finer mesh might have got it running longer.