Another interference fit analysis

[Anonymous]

 Hi All,

There is some great information here on simulating fits, I'm after some help regarding the best workflow for my situation.

I have a cast wheel centre which is supplied with a 90mm bore, I wish to assess the effect of boring out to mount on a 114mm diameter shaft utilizing a 0.1mm interference between shaft and bore. As can be seen in the attached model the centre rim of the wheel has 3-off equi-spaced cut outs and I am particularly interested in the effect of the cut outs under the load applied from the interference fit.

I have used a separation contact between the bore and the shaft with unsymmetric contact penetration type and a maximum activation distance of 0.2mm.

The mesh of these contact surfaces is currently 2mm.

To get even stress distribution from the pressure due to the 0.1mm interference it appears I need a much smaller mesh size - however my PC seems to crash out of the analysis.

I've tried taking a 6o degree "wedge" and apply a radial symmetry based on a cylindrical UCS to reduce model size by 2/3rds however this applied multiple constraint conditions to shared nodes of the shaft so it will not give me a valid solution.

Rather than modelling the interference I tried applying a thermal load to make the shaft expand but I need to research this method further as I could net even get the Nastran file to generate on running the analysis.

Is there any tips anyone could provide to point me in the right direction, also with an efficient simulation set up how long would I expect such a simulation to take with a current midrange i7 CPU +32GB ram (minutes, hours, days??)

Sorry about the long post!

[shigeaki.k]

Hello @Anonymous,

press-fit is done with the parameter NCONTACTGEOMITER  set to zero. 

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Hi @shigeaki.k,

Thanks for the reply, I forgot to mention that I had set the parameter NCONTACTGEOMITER  set to zero.

As an update on my progress, utilizing a 1.5mm mesh between the contact faces I am able to get reasonable results at my area of focus. The contact stresses and displacements are as expected still variable due to this relatively coarse (with respect to the fit tolerance) mesh density. The solve time is around 7 hrs - I'm interested if this time is reasonable?

As a final note the for the simulation to be valid I would expect the displacements at the hub surface to be close to 0.05mm (ie 0.5 times the interference), my displacements were less than this so I expect the stress in my area of focus is under conservative.

Regards, Michael

[shigeaki.k]

Hello @Anonymous,

I have attached the modified model. The analysis should take about 5min.

1) You don't need to split the volume of the shaft. If you do that, you have to apply bonded contact between these split volume even though it looks like a single part in Nastran In-CAD. I modified the shaft model so that the cylindrical surface is split.

2) I made a cylindrical coordinate system and used it to apply a constraint to stop the contact surfaces from rotating as a whole. There are other ways to do this but this felt like the easiest way. Please note that you cannot use a mixture of coordinate systems for constraints. So I have used the same cylindrical coordinate system for the other constraints. 

3) I applied a very small friction to the contact to stop the hub sliding along the shaft.

4) I used unsymmetric contact with the Shaft surfaces set as the Master.
When the Hub surface was set as the Master, both displacement, stress etc. continued to increase with number of sub-steps i.e. the solution did not converge relative to the number of sub-steps. I will contact the Product Team with regards to this matter.

For the stress values, I would use the probe to obtain the values at the points of interest. For circular/cylindrical surfaces, there is always some mesh interference and because of these you can get some hotspots as nodes are moved to remove these interferences.

Above figure extracted from here.

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Sorry @shigeaki.k for taking a while to get back to you - I have had some time away from work.

I've only had a quick look but the model with the updated constraint and contact conditions definitely solves much quicker!

With your set up I noticed the solution showed that the hub deflection at the interference surface was only around 0.025mm where I would think a converged solution should be closer to the interference of 0.05mm (taking into account there will be some variation due to hotspot nodes as you have mentioned).  I will increase the number of increments and also use a smaller mesh. Thanks once again!

Regards Michael

[shigeaki.k]

Hello @Anonymous,

could you also use symmetric contact? I have having a chat with the product team and the results for press-fit can change depending the master/slave selection. Hence I have been told to use symmetric contact with similar mesh for the two surfaces. 

Regards,

Shigeaki K.

[Anonymous]

Is it possible to view stresses about the cylindrical UCS such that the radial and hoop stresses from the interference fit be easily evaluated?

[John_Holtz]

Yes, the stress results can be viewed in a local coordinate system. However, you need to set that up before you run the analysis. The basic steps are as follows:

1. Create a cylindrical coordinate system.
2. Edit the Solid idealization.
3. Change the Material Axes Coordinate System to the cylindrical coordinate system.
4. Run the analysis.
5. The results "Solid X-Normal", "Solid Y-Normal" and "Solid Z-Normal" will now correspond to radial, tangential, and axial stress directions.

If your interference model takes a long time to run, you may want to try this on a small test model first. I discovered this yesterday when using In-CAD 2019.1. It is probably the same in all versions, but it would be good to check it with the version that you are using.

Let us know if that works.

[Anonymous]

Hi @John_Holtz I ran the pipe simulation as you described, but I got some strange results. 1/4 of the model was taken into account.

Hand calulations gives me Hook stress approx. 40 MPa, while from the simulations I got around 90 MPa. I followed the step you mention beside the fact that I was not able to change the Material Axes Coordinate System - simply I was not able to find it. I change it only in the Idealizations, Constraints & Loads

I enclosed the file if you don't mind taking a look.

Regards, 
Bartosz

[shigeaki.k]

Hello @Anonymous,

can you tell us which equation you are using. You have 20MPa applied in the model and for cylinder hoop stress=(Pressure x radius) / thickness = (20x10^6 x  0.01125m)/0.0025m=90MPa. 

See also Cylinder Stress Wiki.

Regards,

Shigeaki K.

P.S. - for future reference, could you start a new thread for new topic/question? It helps keep the forum organised to one topic per thread for easier search. Would be much appreciated.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

The only difference we have is that I used 5 mm thickness instead of 12.5mm.

Apologize, I will keep in mind to start the new thread. It was realted therefore I decided to ask here. 

[John_Holtz]

Hi @Anonymous

You have the cylindrical coordinate system and Idealization setup properly. That's good!

These items are not setup properly:

1. Constraint 2 on the end of the model is fully fixed and applied to both ends. The hand calculations do not take this into account. Therefore, you should use a symmetry constraint (in the axial = Z direction) on one end and delete the constraint on the opposite end.
2. The mesh may be a too coarse. Either use a finer mesh or use parabolic elements.
3. The model is not a thin cylinder, so there will be variations in the stress results through the thickness. You either need to model a thin cylinder or use formulas for a thick cylinder when doing the hand calculations.

After you change items 1 and 2, the X-, Y-, and Z-Solid stress results will correspond to radial, hoop, and axial directions. The stress results will also be uniform along the length which is what the hand calculations assume.

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!