How to Simulate Spring effect

[Amir_Pakroo]

Hi Guys,

I want to be able to understand and simulate the spring stiffness effects on a complex model set by shafts etc,,, but simplified as below,

sofar this model was from another post and thanks to all members helped me to get to know how to set a pin and moving parts in Nastran,

But my mechanism should include effect of springs too, which I added one spring to below same sample to simplify and understand it better, but no luck so far in my settings!

and if someone could be able to help me to set the spring and motions and forces in proper way will be appreciated... (ASSY File attached)

[Roelof.Feijen · Accepted solution]

Hello Amir,

Welkom to the Nastran forum. The main problem is:

1. You have a constraint applied that hinders the part from moving. Remove the "EDGE TZ MOVE" constraint from your analysis.

2. The bottom of the spring is free floating. Use a connector to attach it to the face.

3. Constraint 10 and the newly created Rigid Connector will control both the common nodes on the edge in the Z-direction. If you model a radius on the inner edges, the constrain and rigid connector will not use the same nodes anymore. Otherwise you will end up with a FATAL ERROR E5019. You could also apply the constrain to another face. That is what I did.

4. A spring stiffness of 2 N/mm is very weak in this case. I have changed it to 2e4 N/mm for testing.

5. There is a warning in the Nastran Output window telling you that you use incorrect material properties. You entered a Shear modulus of 80000 MPa. Nastran calculated value too and warns you that it is incorrect. You can leave the value blank and Nastran will calculate this value based on

If you enter a value for the Shear modulus, that value will be used.  If it is left blank the value calculated by the Nastran solver will be used.

I have attached the modified model.

[Amir_Pakroo]

Thank you Roelof,

Very appreciate for your perfect explain and slowly I'm getting the Nastran concepts and its reasons for the errors,

Just a questions pls, If i change the stiffness of the spring, the displacement value will be shown and changed accurate as below images but seems the contour graph of the movement will be shown same in both situations,
Is it normal in Nastran or I'm missing something here ??

(One image related to K1: 100/16mm another K1: 2000/0.8mm)

Also regarding the error for shear Module do you mean when I choose any standard material for each solid then I have to change it to blank ? in below dialog box you mean ?

[Roelof.Feijen · Accepted solution]

Hello Amir,

The displacement results in a linear static analysis is set to 10 percent. It's not the actual displacement. Displacements in a linear analysis are considered to be small. So to see the deformed shape of your model the displacement is scaled. 

When you richt click on the Deformation Plot in the Nastran Browser and choose Edit you can change this in the Deformation Options to actual.

When you select a material from one of the material libraries the value for Shear modules is ignored. So the field will be left blank by default. This was changed, I think, from release 2018. So if you are running an older version you can clear the input for Shear modulus (G). In newer versions this is no longer necessary.

[Amir_Pakroo]

Appreciate Roelof for your helps 👍