Learning Forum

[cristian.pujol]

Hi

I have done a non linear analysis with with a bilinear isotropic hardening. Steel is S690 yield stress 690MPa Ultimate 770MPa

I have used bonded contact to represent the weld on diferent parts, what is bothering me is that there are zones higher than the ultimate stress 770MPa and I think it's due to the bonded contact, i think the bonded MPC contact should be used only with linear materials, but not sure.

What type of contact or furmulation should I use when doing a non-linear material calculation

Thanks in advance

Cordial greetings

[peteroznewman]

It is best to avoid using Bonded Contact with non-linear materials anywhere near locations of high stress or high stress gradient.

Instead use Shared Topology by clicking on the Share button on the Workbench tab in SpaceClaim.

Even after doing that, it is still possible for stress in an element to exceed the ultimate stress of 770 MPa.

What did you use for the Tangent Modulus for the Bilinear Hardening slope? That slope continues along the strain axis to infinity so 770 MPa is just one point along that slope. If the load continues to increase, the stress continues to increase.  What you can do, after you removed the bonded contact, is to note the simulation time when the 770 MPa is reached and note the load when that occurs as the Ultimate Load.

One other problem is extrapolation of stress from the internal Gauss points out to the corner nodes. When the elements are large, that can cause a significant increase in the reported stress. Make sure to use smaller elements in the region of high stress to reduce this problem, and/or insert the Command ERESX,NO into the model to copy instead of extrapolate stress to the corner nodes.

[cristian.pujol]

Thanks for you're answer 

The problem with shared topology is that i can't use it because i have two materials, the big tube is S355 and the other tubes S690

For S355 I used Yield stress 350 MPa and tangent modolus of 2100MPa

For S690 I used Yield stress 690 MPa and tangent modolus of 4140MPa.

So in this case where we have two materials what would be the procedure for "gluing" the two tubes?

 

Thanks in advance for the answer

Regards

 

[Myles.Washburn]

"The problem with shared topology is that i can't use it because i have two materials"

It is not clear to me whay you say this.

It is not recommended to use bonded contact in an area of interest.  

Use the 'shared topology' tools to connect the bodies together, the nodes will be merged etc.

Indeed meshing can be more challenging, but this is what is required.

Use linear elements.

Averging of results across bodies can be turned on/off if desired.

[peteroznewman]

Myles is correct, using Shared Topology maintains separate bodies that can each be assigned a unique material.  In that way, it is different to using a CAD unite command to merge mulitple bodies into a single body.  Shared Topology creates a multibody part.

When using Linear elements, make sure to use at least 4 elements across the thin dimension of any body in the part.