Dear community,
I am having trouble with modelling a press fit. Below you can see a sleeve (yellow) that is applied by a press fit onto the shaft (red). The picture shows a cut through the symmetric model. In Inventor professional I would simply make the sleeve a bit smaller and apply a shrink fit with no sliding contact. As a result I would then see the defomation of the sleeve and the shaft. How can I achieve this with Nastran in-Cad?
I would really appreciate any help.
Kind Regards
Santino Keusemann
P.S.: In case someone wants to model this with actual numbers, the shaft diameter is ø260 mm and the sleeve will be 0,26 mm smaller.
Hi Santino Keusemann,
Welcome to the Nastran In-CAD forum! Interesting question you have there, I had to do a bit of research myself on this. With a physically modeled interference you will need to use a non-linear static solution. Once you've defined your separation contact between the two surfaces in question we will need to make one change to the the Nastran Parameters, these can be found at the bottom of the model tree. Simply right-click and Edit, go to Non-linear Solution Processor Parameters and check the Advanced Setting checkbox. You will then want to set NCONTACTGEOMITER to 0, this will cause the solver not to move around the contact elements that already have interference detected. With these settings you should be able to observe your interference fit with Nastran In-CAD.
Regards,
Andrew
Hi Andrew,
thank you very much. I will try it as soon as possible. This week I will be on business travel. Afterwards I will check it.
Mit freundlichen Grüßen / Best regards
Dr.-Ing. Santino Keusemann
Dear Dr.-Ing. Santino Keusemann,
I have tried to model a similar problem. Did you get your model to run successfully?
Robin
Hi Robin,
Are you having a problem with an analysis? If so, I suggest that you create a new post and describe your analysis, such as
I will carry on this thread for the moment since I am doing a similar thing and I tried the solution above with no success.
This is the error I get: FATAL ERROR T2135: UNABLE TO GENERATE SURFACE CONTACT USING SPECIFIED PARAMETERS
In the model from 50h9j, the warning occurs because the solver cannot find any nodes on surface 1 that are "in the plane" of surface 2. By default, it is looking for nodes that are 0 mm apart.
Since the model includes the interference fit of 0.1 mm, the surfaces are initially "separated" by 0.1 mm. You need to enter a "Max Activation Distance" on the surface contact setup that is larger than this distance. A value of 0.2 mm will work. See the attached image.
John, thanks for that simple but critical solution.
Robin
John,
I have done another very similar simulation but this fails with an E5000 error.
Would you mind taking a look?
thanks
Robin
Hi @50h9j
Strange. I ran your model (RotorStar 4962-500kv motor.zip) but did not get any errors. There was one part missing from the assembly (RotorStar 4962-500kv.ipt), so that may have been the problem if that part was included in your analysis.
In general, I would agree that having parts in a static analysis that are not statically stable can be a problem. For this particular model (a pulley on a shaft), I would not get too fancy with trying to model the connection between the grub screw (set screw), pulley , and shaft. Instead, I would apply a constraint at the bottom of the screw hole to hold the pulley in the axial direction (Z direction in your model).
If you were doing an analysis with an axial load on the pulley and therefore needed the effect of the screw to hold the shaft, I would probably use a Connector > Bolt to model it. In that case, you would want to make some modifications to the CAD model by splitting surfaces in the region of the screw.
There are only 2 parts in the analysis. I think the missing part derives the shaft.
I have put a constraint on the bottom edge of the hole in the z-direction as suggested.
I also found that the interference contact was asymmetric so I changed that.
It now solves in 10 increments. The internal surface of the plastic pulley is pock-marked while the steel shaft is smooth. I realise this is highly magnified but it seems to indicate a poor quality solution. It does not give me much confidence that applying a torque to the pulley as well will give accurate results.
I wondered about modelling a segment but was not sure how torsional deflections would be handled. I suppose I could slice it using x-y axis planes and ignore edge effects.
There shouldn't be this asymmetry in a press fit?!
I tried a 2mm slice then I tried mid-planes using a 0.1mm slice. Finally got it to solve for bonded and separation contact as a linear static analysis.
Not sure why separation result gives an overlap. Still won't solve as a non-linear static analysis.
Neither have an interference fit. I couldn't get that to work with the mid-plane idealization.
separation contact 1:1 scale displacement