Sliding surface stiffness (Need urgent help)

  • 67 Views
  • Last Post 3 weeks ago
  • Topic Is Solved
AbdulBasit03 posted this 3 weeks ago

Hi ,

I have modelled a Linear feed drive system , since the linear roller bearing  translates in axial direction The stiffness of the bearings are always directed along the line containing the point of contact of balls . Since these points move as the bearing moves stiffness cant be defined by a longitudinal spring that is only connect to nodes which elongates as bearings moves  , the stiffness should be consistent as the system moves . What is the best way to do that in ansys? I see an option in solid works called flat parallel faces .

This picture titled  (spring)  shows a spring between the bearing the guide , as the bearing moves the spring elongates . I do not want this I want the spring to move as the bearing moves to maintain the same normal stiffness.

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 3 weeks ago

I recommend you delete the springs and add a No Separation Contact between the carriage and the rails.

If you want detail, you can define that between the ball and the race.

What I usually do is simplify the rail and carriage so there are two or three flat faces that define the carriage to rail No Separation contact faces.

You can adjust the contact stiffness if you feel you need a stiffness in the model that matches the manufacturer's specification.

  • Liked by
  • AbdulBasit03
AbdulBasit03 posted this 3 weeks ago

Hi

I have removed the springs , I already have a frictional contact that has the coefficient of friction of the linear bearing . Now I added no separation as well . The problem is I am trying to update the normal stiffness in the worksheet using contact tool , every time i put the values and generate initial information it puts the normal stiffness back to 0 in no separation  contact . 

In between the guide and the linear bearing do I need ''a translation joint that gives it one degree of freedom'' a frictional contact with coefficient of friction and a no separation contact with normal stiffness as that of the linear bearing balls as I have put all three of them . ? Can you please guide me on how to manually put the normal stiffness of 600000000 N/m.

Thank you 

Abdul Basit 

peteroznewman posted this 3 weeks ago

It would be easier to guide you if you use the Attach button to upload a Workbench Project Archive .wbpz file.  Make sure the file is < 120 MB.  Delete the Mesh to make the file size smaller.

  • Liked by
  • AbdulBasit03
AbdulBasit03 posted this 3 weeks ago

  Hi ,

Please find the attached Analysis file .

Thank you 

 

peteroznewman posted this 3 weeks ago

Where?

  • Liked by
  • AbdulBasit03
AbdulBasit03 posted this 3 weeks ago

Unfortunately the file is too large  , even after deleting the mesh and archiving its 238 mb. Can the attached pictures help ?

Attached Files

AbdulBasit03 posted this 3 weeks ago

In the pictures above , The no separation connection may be not be visible but it follows the same problem, when i put the Normal stiffness values in these yellow boxes they dont remain there they turn back to zero when i update initial information . both for friction and for the no separation . I have even changed the parameters from program controlled to manual nothing happens it just tells me to give an normal stiffness factor which i dont know how to relate to normal stiffness of 600000000N/m.

peteroznewman posted this 3 weeks ago

You can make the 238 MB file available using your Google Drive.

If you have a Gmail account, and you attach that file to an email, it will upload the file to your Google Drive and provide a link in the email.

Copy and paste that link into your reply and I can download it from your Google Drive.

  • Liked by
  • AbdulBasit03
AbdulBasit03 posted this 3 weeks ago

Can you Find it here?

[link removed]

AbdulBasit03 posted this 3 weeks ago

Its a bit confidential please can you delete the link once downloaded ? Also can you confirm if its working

peteroznewman posted this 3 weeks ago

Okay, I downloaded the file and will have a look later today.

  • Liked by
  • AbdulBasit03
peteroznewman posted this 3 weeks ago

I recommend you delete all the Frictional - GUIDE RAIL contacts because they interfere with the Translational - GUIDE RAIL joints that do what you want.

  • Liked by
  • AbdulBasit03
AbdulBasit03 posted this 3 weeks ago

I have supressed them , but i am still unable to update the normal stiffness value of the no separation contact in the contact tool , it doesnt change . Did try changing the normal stiffness ? it always remains at 1.9074 e+014

Attached Files

peteroznewman posted this 3 weeks ago

I also recommend you delete all the Translational Joints as well because they interfere with the No Separation contacts (which I didn't see before).

I recommend you merge the two No Separation contacts on the same rail into one contact with two carriages and flip the Contact/Target scope.

You can override the Normal Stiffness Value, but I don't recommend it.

 

  • Liked by
  • AbdulBasit03
AbdulBasit03 posted this 3 weeks ago

Okay ,  I will do that , In reality the balls of carriage have a stiffness of 600000000 N/m and a coefficient of friction of 0.025. Also the joint translates . Would all these conditions be met by no separation contact? I see there is no friction in no separation contact and you recommend not to keep the stiffness too would that not deviate from real boundary conditions ?

 

Thank You 

peteroznewman posted this 3 weeks ago

Look at the Normal Stiffness Value, it has units of N/mm^3.  You have a stiffness with units of N/m.  You would need to know the area of the contact that ANSYS is using in order to convert the stiffness you have to the stiffness you have to enter into ANSYS.

Once you see how mode 1 and mode 2 moves, you will see that the stiffness of the bearings will have no practical effect on the frequency or mode shape of modes 1 and 2.

Modal analysis uses only frictionless No Separation contact. It cannot include friction because it is a Linear analysis.

  • Liked by
  • AbdulBasit03
AbdulBasit03 posted this 3 weeks ago

Hi Peter, 

 

Great Stuff , Thank you so much for your help greatly appreciate your time Sir. Pardon me for asking too many questions . Thanks again. 

 

 

Abdul Basit

Close