UGNX Nastran 7.5 2D Axis Symmetry Problem with 1D Spring

[thecadguy]

Dear All,

I am running a 2D Axis Symmetry Problem, with contact, and everything is running good. However, I need to use a spring and there is no 1D elements available? Are you kidding me! Can anyone shed some light on this why and also what would be a good work around fix.

Thanks,

The CAD GUY

 

[BlasMolero]

Hello!,
I understand you are running NX Advanced Simulation, not FEMAP, in this case the option choosed of "ANALYSIS TYPE = AXISYMMETRIC STRUCTURAL" is mandatory, you say that you want to run a Axisymmetric analysis (solid of revolution) where the study of 1-radian is perfect as both loads & geometry repeats constantly in 360º, then the finite elements available are 2-D Solid TRI/QUAD elements.

Here you are a 2-D axisymmetric analysis with contacts:

In NX AdvSim the workaround is to study say 1/4 model, prescribing the symmetry boundary conditions in the planes of symmetry. Here you are the same problem in 3-D, results are exactly the same, but you pay the tickect of solution time & model size:

Using FEMAP you are free to mix 1-D elemets with 3-D or 2-D elements, not limitation, .....
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[thecadguy]

Thanks for the reply. Two questions.

Could I simulate a spring with shell elements and adjust the material properties for stiffness.


If I do do a 3d 1/4 model how would I simulate the inital compression of the seal. In 2d it is a linear movement. In 3d it would have to be a radial movement which how to do with an enforced displacement?

 

[BlasMolero]

Hello!,
1.- In a general model yes, you can mix 1-D Spring CELAS2 elements with 2-D Shell CQUAD4 elements. The spring element's stiffness is introduced directly in the spring element definition property & connection card, is not related with any material property, only applies to PSHELL element property card that defines the membrane, bending, transverse shear, and coupling properties of thin shell elements using material identification numbers MID1, MID2, MID3 & MID4:
• MID1: Material identification number for the membrane stiffness.
• MID2: Material identification number for bending stiffness.
• MID3: Material identification number for transverse shear stiffness.
• MID4: Material identification number for membrane-bending coupling.

2.- You can prescribe an enforced displacement using any cylindrical coordinate system, where DOF2 means radial direction.

To understand better your problem is best to plot a sketch or diagram of the model with loads & constrainst, a picture is better than 1000 words.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Frawol]

Hello!

I think you are able to generate axissymmetric nastran input files containing 2D AND 1D elements exported from the NX Advanced Sim. To get this file is tricky and not very user friendly, furthermore knowledge of the nastran language would be helpful I would say.

You have to edit the input file "by hand" before sending it to nastran. In the .fem, when the axissymmetric solver is acitve you can't genarate 1D elements. So you have to do this when the analysis type is switched to structural on the same model. Afterwards, you have to export the element (and possibly node) definitons (which can't be build in axissymmetric analysis type) into a text file (is the model very simple you can modify the nodes and elements definitons in the dck file directly without this detour). When not already done, switch back to axissymetric and build the 2D elements.

Before solving the axissymmetric solution you have to add the txt file containing the 1D bulk data definitons to the axissymmetric .dck file. There are several ways to do this (copy/paste by hand; import via "user defined text", ...).
At this point you must be carefully, not to get contradicting element and node definitions. If you want to apply loads to the 1D elements you have to add this definitons to the dck file by hand as well.

For better understanding take a look into the Nastran Users Guide and find out the difference between the structural and the axissymmetric structural analysis. The differences are comprehensible and there are only few points to take special care.

Regards,
Franz

 

[thecadguy]

Dear All,

Thanks for the response. I have decided to invest in FEMAP to get the job done because of the lack of functionality in UGNX advanced simulation. I still can't believe they omitted such a basic 1D element in the pre-processor especially since NX supports the solutions.

However, I do have a question regarding the time steps for this 2D axis symmetry problem. I will try and break it down and get some comments on whether I should use single or multiple intervals. I have tried both and can not seem to get it to work correctly.


Geometry: O-ring in O-ring Groove to seal a piston in a housing. (Simple)

Total Time: .05 step time over 20 steps for a total of 1s

Step 1: I need to simulate the seal so it is in its compressed state because in the free state the seal intersects thru the groove if i keep the seal tangent to the piston. The technique I use is to take a portion of the elements around the housing groove (tool0 and move the 2D elements away from the centerline to give enough clearance to the seal. It is about .5mm. No I apply an enforced displacement of this "tool" and compressed the seal to a position as installed. The tool elements are identical to the housing groove elements. I apply the enforced displacement using a table with the following:

0s,0mm
.5s,.5mm
1s,.5 mm

So essentially the seal gets compressed within the first .5s and stays there. This works great with a single load. The problem is when I introduce a second load after the initial seal compression.

Step: 2: I apply a pressure on the crown of the piston which will induce a linear axis movement of the piston and cause the side wall of the piston to pull or tug at the compressed interface with the installed seal.

The pressure is applied:

0s,0 MPA
.5s,0 MPA
1s,20 MPA

If I apply just the pressure load it works fine but when I combine the load it appears both loads are being applied at the same time instead of a stepped manner?

I am trying this approach because of only one subcase allowed in sol 601. I do not know of another way to try and apply loads in series other than vary the time application? I eventually want to apply the same pressure to the back side of the seal but have not gotten that far.

What I notice sometimes is that the solution will stop at the .5s mark and not even get to apply the pressure load. I would appreciate any thoughts to timesteps and load applications?

THanks,

CADGUY

 

[thecadguy]

All,

Regardless of adding a time step to the enforced displacement I get the feeling NX does the enforced displacement first before any of the other loads? If this is true than How would I add an enforced displacement say at around .5s of a 1s solution? When I do add the enforced displacement to end at the .5s mark of a 1s solution the solution stops at the .5s and doe snot continue to 1s even though I have a pressure load that starts at .5s and goes to 1s.

The CAD Guy