cancel
Showing results for 
Search instead for 
Did you mean: 

Contact analysis in SOL 601

Valued Contributor
Valued Contributor

Hi,

I have analysis a bolted connection using SOL 101, including contact. This works fine.

 

However I  would like to investigate the problem using SOL 601 with material non-linearity in combination with contact. Problem is that the solver not includes the contact as defined in the SIM file (face contact) in the analysis. No contact pressure is reported. The "Face contact" is included to the Solution in the same manner as for the linear SOL 101 analysis.

 

Most likelly a very easy question for the experienced SOL 601 user: Any settings typically overlooked for the contact to be included in the SOL 601 analysis?

 

Best regards

Geir Olav Guddal

5 REPLIES

Re: Contact analysis in SOL 601

Siemens Phenom Siemens Phenom
Siemens Phenom

In SOL 101, initial contact stiffness is added at the start of the solution, prior to loads being applied. This works to stabilize components that are grounded only by contact.

 

In SOL 601, contact is detected after the initial loads are applied. You may need an initial time step or two with zero or very small load magnitudes to allow contact to establish. After contact is established, loads should be ramped up to their full magnitude.

Re: Contact analysis in SOL 601

Valued Contributor
Valued Contributor

Thanks Jim,

 

I have stepped up the load as shown:

Load step.jpg

 

The SOL601 analysis works fine with respect to the material non-linearity,  but I am not able to establish contact using thin shell. See plot below. The deformation shape is not correct.

 

SOL601 2D.jpg

 

 

 

 

 

 

 

 

 

I tried a 3D mesh with parabolic brick elements. Contact was then established in the SOL 601 analysis. See deflection plot below. Note that symmetry is used to reduce the size of the problem:

 

3D3D

 

 

 

 

 

 

 

 

 

 

My question is now if contact analysis is supported in SOL 601 using thin shell elements? – or are there any special settings to be used?

 

Best regards

Geir Olav Guddal 

Re: Contact analysis in SOL 601

Siemens Phenom Siemens Phenom
Siemens Phenom

The only difference between using shell element faces and solid element faces is that the contact side (top or bottom surface) must be specified for shell faces. The top face follows the element positive normal.

 

Top is the default, so you probably need to change one or both regions to bottom to be defined correctly.

Re: Contact analysis in SOL 601

Valued Contributor
Valued Contributor

I think the definitions of top and bottom is OK. Please note that the contact analysis works fine when using SOL101, I only have this problem in SOL601. For your information I attach a plot from the SOL 101 analysis:

 

SOL101 2D.jpg

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

I will try the official Siemens support system to see if they can find the reason for my problem. If being of interest in this forum I will let you know the outcome.

Thanks for your comments anyway Jim!

 

BR

Geir Olav Guddal

 

Re: Contact analysis in SOL 601

Valued Contributor
Valued Contributor

Hi,

 

The suggestion from Siemens was to initiate the programme to automatically calculate and use half of the thickness. To obtain this it was proposed to use BCTPARA - Contact Parameter - and to input "Half the thickness" to the Standard Contact Algoritm.

This suggestion did not solve my issue.

 

Luckilly I got a private suggestion in the community, proposing to input half of the shell thickness manually. In my case with a 25mm plate:

SOL601.jpg

 

This solved my problem.

 

Note that the similar input when running the initial linear elastic analysis in SOL106 requires the offset to be zero. The effecth of the half the shell thickness is then calculated automatically.

 

To me the above does not seams properly described in the NX help system.

 

Best regards

Geir Olav Guddal