How can I constraint pins and bushings?

  • 86 Views
  • Last Post 3 weeks ago
LuisGil posted this 3 weeks ago

Hi there!

I'm designing a mechanical knee prosthesis (optimal design), and i can't constraint the axial movement of the pins.

Contacts between bushings and pins are no separation, bushing and links are bonded, links and solid faces of upper and lower pieces are frictionless (because i need to simulate the buckling load factor). 

A remote force of 2013N (ISO 10328) was applied in the bottom face and a fixed support in the upper face.

Any suggestion?

Attached Files

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

Hi LuisGil,

If you attach an archive of your model, it will be easier to see in detail what you have and make suggestions. To create an archive in Workbench, Clear Generated Data on the Model item and save the Project.  Then click File, Archive... and save a .wbpz file.  You can use the Attach button to your first post to upload that file if it is < 120 MB. Please edit your post and add which version of ANSYS you are using (17.2, 18.2 etc).

You say you need to simulate the buckling load factor. Does that mean you have a Static Structural model that solves?  Is the line of the remote force pointed up in a stable direction?

You also say "I can't constrain the axial movement of the pins."  Do you mean you tried to do it and ANSYS wouldn't allow it, or that you don't know how to?

The bushings are bonded to the links, is that because they are a press fit?

What is the ID of the the bushing?  What is the OD of the pin?
If there is a clearance, is the centerline of the pin coaxial with the centerline of the bushing?
That would be typical of most CAD design layouts, but is not appropriate for analysis.
In the figure below, I show (exaggerated) a hole that represents the ID of the bushing and the pin.


What you want for analysis is for the clearance between the parts to be taken up in the way they would be in a physical sample under load (reality).

The buckling load will be sensitive to the location of load paths through the parts and it matters if the load is on the inside or the outside of the thickness of a part.

 

  • Liked by
  • LuisGil
LuisGil posted this 3 weeks ago

Hi peteroznewman! 

I´m using Ansys 18.1, there are the files of my WB project attached.

I need to solve a eigenvalue buckling analysis, but I couldn´t solve the static structural analysis because i can´t constraint the axial movement of the pins and links properly. I tried many ways to do it but I don´t know how to.

ISO 10328 describes two load conditions, where the compression forces are asymmetric. 

 

this is an example of the load condition 2.

The bushing contacts are bonded because the are a press fit (ID of the links are 12mm and 10mm and OD of the bushing are 11.98mm and 9.98mm)

The centerline of the pin is coaxial with the centerline of the bushing and links.

The clearance between bushings and links are 0.1mm.

peteroznewman posted this 3 weeks ago

I don't see an attached .wbpz file.

I have found the Attach function is a bit broken.

When I first try, and I have to use browse to change folders to get to where the .wbpz file is, the upload doesn't start.

The workaround is to refresh the browser page and click Attach again. This time, when I click browse, the file is there without having to change folders and the Upload button works.

Is that what you found?

LuisGil posted this 3 weeks ago

I uploaded it again, try again please.

peteroznewman posted this 3 weeks ago

I suppressed all the pins, shafts and bushings and was left with a 4-bar mechanism. I created a revolute joint at each pin location.

This model has no static solution because it is a mechanism. If one of the joints is changed from a revolute to a fixed joint, then there is a static equilibrium solution.

Arbitrarily changing a revolute to fixed is not correct. There must be a locking mechanism that keeps the knee joint locked in the straight position. In the image below I see a center link connecting two shafts and a telescoping pair of parts. I expect there is a heavy spring (not shown) between the telescoping parts.

 I can add these parts in and a spring, then there will be an equilibrium position with the remote force. I took some shortcuts by using joints that had one side along the whole length of a shaft. If I was doing this more carefully, I would replace the joint with contact, or split the face so that only the portion of the shaft touching the other part is part of the joint definition. But at least this quick model shows the elements needed for a static solution. Note that I turned on Large Deflection in the Analysis Settings.

 

The center spring is supporting a 10,275 N tension force.
The bottom of the knee swings forward about 15 mm under this load.

The Eigenvalue Buckling system will solve, but the solution has large negative Load Multipliers. 

 

Attached Files

LuisGil posted this 3 weeks ago

What you pointed out in this image is the Knee-Extension-Assist System. In the straight position, the KEA System will not exert any force, because the spring is in free position, that´s why I supressed that system in the analysis

.

There is no locking mechanism. The Prosthesis has a blocking stop as you can see in the image below. It was modified to improve the contact surface.

So you suggest that I supress the pins and bushings in the static analysis? Is that correct?

I couldn´t open the file that you attached because it was modified in a new version of ansys. I use Ansys 18.1

peteroznewman posted this 3 weeks ago

A good strategy when model building is to get the simplest possible model running first. You will learn 80% of what you need to know from the simple model. Then you can build a refined model to fill out the remaining 20% of the information. Of course you will spend 80% of your time building the refined model after only having spent 20% of your time on the simple model. By suppressing everything but six parts and creating eight joints plus one contact, you can solve the statics problem. That took me < 10 minutes before I could hit solve.

Now I see the stop, I should have noticed that before. I added frictional contact between the links and stop and used Adjust to Touch to close the small gap. I dragged and dropped the contact onto the mesh to create mesh refinement at the contact point, then I added a Face Sizing mesh control on the stop face. I turned Large Deflection on and turned on Auto Time stepping. Now the Static Structural model solves.

Unfortunately, the Maximum Equiv. Stress is much greater than the Ultimate Tensile Strength of Aluminum Alloy, which is 310 MPa. It is clear that this load will cause the stop to fail. Does the solution to the Eigenvalue Buckling problem even matter after learning this?

I used ANSYS 18.2 for the attachment above. I have attached a redo in ANSYS 18.1 format to this reply.

Attached Files

Close