Discussion Groups

Simulation Mechanical and Multiphysics

Reply
Contributor
jm74jensen
Posts: 12
Registered: ‎06-18-2008

Shrink Fit in Simulation Mechanical

365 Views, 4 Replies
03-13-2013 12:34 PM

I have applied Shrink Fit/Sliding between the bore of a hub and the OD of a shaft. I have included 0.0045" interference between the surfaces and a 1.0 friction factor. The results show the surfaces move relative to each other but there is some sort of local loading between two pairs of nodes that appear to be tugging on each other. I have tried both part-to-part settings as well as surface-to-surface settings. On previous versions of this model, I obtained results that did not exhibit this sort of erroneous action. This is causing an inappropriate extreme level of stress. What would explain this sort of behavior?

Please use plain text.
Valued Mentor
AstroJohnPE
Posts: 510
Registered: ‎08-30-2012

Re: Shrink Fit in Simulation Mechanical

03-13-2013 06:29 PM in reply to: jm74jensen

Hi,

 

I have a few questions about your image.

  •  If I understand correctly, parts 2 and 4 are in contact. What type of contact is between the parts/surfaces at that location?
  • It looks as if the mesh on parts 2 and 4 are different. (Actually, it looks like they are very different.) Is this true? Or do they look different because of the displacement scale?
  • What is the analysis type?

I thought that the only type of contact that can handle different meshes on the "matching" surfaces is bonded contact, and only when "smart bonding" is activated. This can cause "hot spots" in the stress results.

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.
Contributor
jm74jensen
Posts: 12
Registered: ‎06-18-2008

Re: Shrink Fit in Simulation Mechanical

03-14-2013 06:10 AM in reply to: AstroJohnPE
Thank you for the response. The analysis type is Static Stress with Linear Materials. The meshes match in a large portion of the surface area. There are unmatched area toward the edge with the finer mesh. The earlier images were of the deflected shape. The following images shows the un-deflected surfaces on top of each other. One is highlighted (yellow) the other can be seen as black where it is not matching. You can also see here that the two pairs of nodes appear aligned to each other. The nodes do share common XYZ position as shown in the earlier results image. The mesh lines appear to align better before I add refinement points. Should I be adding refinement points to both parts. I was thinking that their sphere or radius of influence would cause a matching effect on both of the mating parts and it indeed appears to have done this. [cid:image004.jpg@01CE2093.C07BE730] In the following image, the opposing surface is highlighted. [cid:image006.jpg@01CE2093.C07BE730] I had run a couple different versions of this type of condition and did not obtain such hot spots. I have been trying different surface contact types. On earlier models I started with "Surface Contact", then "Shrink Fit/Sliding" and then "Shrink Fit/No sliding". In the earlier models I was getting results that appeared as one might expect. I had redesigned the part(s), re-meshed and so-forth and this sort of hot spot result began to appear. The following images are from an earlier version of the model. They show a similar mesh mis-match in the refined area, but this model did not exhibit such a hot spot in the stress distribution. I had set the contacts to the three types in different scenarios and they each came back without this type of hot spot. What I am attempting to model is the interaction of a steel gear hub with a press fit (shrink fit) onto a matching steel hub. A key is used to transmit torque loading. The effect of pressure on the keyway edge appears to be my current area of concern. Other critical areas of concern of the hub design have been redesigned to develop an acceptable level of stress. The actual loading on the key is subject to the potential slip between these two surfaces. In reality the fit may be sufficient to transmit the torque, but the level of actual fit can be a bit unknown and therefor the share of load taken by the key is somewhat unknown also. I would like to vary the fit and friction factor to study their effect on the stress level at the keyway edge. [cid:image009.jpg@01CE2093.C07BE730] Again, this is the opposite surface highlighted. [cid:image013.jpg@01CE2093.C07BE730] While we are discussing this model, I am looking for advise on element types, ie, "bricks and tets" versus "all tets". The solid meshing under the "bricks and tets" option takes so much longer than the "all tets" option. Which would be most appropriate when modeling solid steel shafting fitted to other soild components as well as other types of interconnected somewhat thick steel sections? I have modeled the components in Inventor with zero gap between the surfaces. What steps can I take to better assure that the surface mesh matches more closely? Regards, Jay May Engineer Engineering | Morgan Engineering 330-823-6130 x268 1049 South Mahoning Avenue Alliance, OH 44601 [Description: Description: Description: Morgan Engineering]________________________________ THIS MESSAGE AND ANY INCLUDED ATTACHMENTS ARE INTENDED FOR THE SOLE USE OF THE INDIVIDUAL OR ENTITY TO WHICH IT IS ADDRESSED. THE INFORMATION CONTAINED HEREIN IS CONFIDENTIAL, PROPRIETARY OR PRIVILEGED AND MAY BE SUBJECT TO PROTECTION UNDER LAW. YOU ARE NOTIFIED THAT UNAUTHORIZED USE, DISTRIBUTION, REVIEW OR REPRODUCTION OF SUCH INFORMATION IS STRICTLY PROHIBITED AND MAY SUBJECT YOU TO CRIMINAL OR CIVIL PENALTIES. IF YOU HAVE RECEIVED THIS TRANSMISSION IN ERROR, PLEASE PROMPTLY DELETE IT AND NOTIFY THE SENDER BY E-MAIL. ALSO NOTE THAT THIS FORM OF COMMUNICATION IS NOT SECURE; IT CAN BE INTERCEPTED, AND MAY NOT NECESSARILY BE FREE OF ERRORS AND VIRUSES IN SPITE OF REASONABLE EFFORTS TO SECURE THIS MEDIUM.
Please use plain text.
Contributor
jm74jensen
Posts: 12
Registered: ‎06-18-2008

Re: Shrink Fit in Simulation Mechanical

03-14-2013 07:54 AM in reply to: jm74jensen

here is a PDF file of my message with th images included

Please use plain text.
Valued Mentor
AstroJohnPE
Posts: 510
Registered: ‎08-30-2012

Re: Shrink Fit in Simulation Mechanical

03-15-2013 11:56 AM in reply to: jm74jensen

Hi Jay,

 

It does look like there is some mismatched mesh. To clarify one statement I made before, there will be contact between nodes that are matched on the two parts (same physical coordinate) but no contact where the mesh is not matched. Obviously, this later situation does not match reality. I do not have a suggestion about the matching other than trying your suggestion of an all-tet mesh. (You may even want to redo one of the previous models with all-tet and compare the results.)

 

One solution that may help the hot spots is to right-click on the contact listing in the browser and choose "Settings". Change the "Surface contact direction" to "Normal to the first part/surface" or to the second part/surface. I think the hot spots are due to the contact elements being crooked where the mesh transitions from matched to unmatched. Of course, these hot spots are a secondary concern -- the first concern is getting the mesh to match.

 

When ever working with surface contact, you should always check the "Results Contours > Other Results > Element Forces > Axial Forces". This will show what the contact force is, but more importantly, it will show where there are no contact elements (because there will be no contour in that location).

 

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Please use plain text.