Showing results for 
Search instead for 
Did you mean: 
Showing results for 
Search instead for 
Did you mean: 

Community Tip - Need to share some code when posting a question or reply? Make sure to use the "Insert code sample" menu option. Learn more! X

Ball Joint in Mechanica


Ball Joint in Mechanica

Is there any turn around for Ball Joint in Mechanica?

I searched the forum, but couldn't find, All I see were related to Mechanism

I need to do a validation on the steering arm, which transfers the load from the Ball Joint to King Pin.

Pls anyone show me some light to simulate the Ball Joint or how this mechanism can be handled

Image Courtesy: Wikipedia.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

It depends on exactly which component you want to analyse.

Do you care about the stresses within the ball joint itself, or only a component that it's attached to?

Usually, I think a weighted or rigid link, or even a Total Load at Point, should be sufficient to apply the loads into the component under analysis.

I forgot to give few info,
I'm using Creo1.0 on XP I'm all the way new to it.

I'm not sure how the advancements actually work like rigid link(DOF)

And answering to your question,

My concern is to study only the Steering Arm, but I want to simulate the Ball Joint as well.

I've directly applied the load to the center of the Ball Joint and excluded the outer cover, but my results seems to be multipled(I mean load on steering arm seems to be) So I like to simulate the Joint now to get closer to real.

Your first approach sounds like the right one to me.

How exactly have you applied the load to the ball joint? Can you share the model, or at least screenshots? What makes you think the load is multiplied?

I couldn't share the Screen shot for now,

I'm comparing the results with ANSYS results.

The results are almost 1.5 to 1.8 times more in Mechanica.

That is what makes me think its multiplied.

If you're looking at stress values, I think it's more likely to be due to differences in the mesh and the solving equations (P-element vs H-element). Is the Ansys model fully converged (if you use a finer mesh, do the stress results change)? For simple geometry, Mechanica is often very good at automatically finding the required accuracy.

There is a very useful function in Mechanica called Review Total Load. In WF it's under the Info menu; I'm sorry, but I don't know where it is in Creo 1. This will confirm the resultant forces and moments acting on your model about a chosen coordinate system.

Thanks Jonathan,

I just checked with the person who done the Analysis in Ansys.
I'll let you know once I do one more run here..

My questions would be:

How did they simulate the connection in ANSYS?

Where are you reading results that give you the 1.5 - 1.8X multiplier?

Without seeing some screen shots and more details of what exactly you are trying to accomplish, it is tough to answer your question.

Basically, if you understand how the joint was set up in ANSYS and, as Jonathan stated, both answers are converged solutions (with a reasonable mesh in Mechanica), you should get correlation. I was corporate support for Mechanica for many years, and I handled many "Mechanica is wrong" calls only to show that when you have an apples-to-apples model between the two different pieces of software, you will get answers that are similar well within reason.

If they are using a spherical joint from ANSYS Workbench, it should just be a matter of finding out what options they used in ANSYS (rigid or deformable) and then applying a similar set of weighted or rigid links with advanced DOF control in Mechanica. The deformable option in ANSYS might be tricky to replicate with a weighted link in Mechanica, as ANSYS allows surfaces on both sides of the connection while Mechanica allows only a dependent point.

Keep in mind though that the conditions right at the joint (where weighted links or rigid links are applied) probably will not be useful for extracting peak stresses. If you need stresses at the joint interaction, you will likely need to simulate full contact conditions.

There are sometimes limitations that keep you from creating an applies-to-apples model, such as if you were to use frictional contact in ANSYS, as that capability is not available in Mechanica. However, over the years in linear analysis, I was able to find a reasonable compromise most of the time for different features between software packages that would produce similar answers.

When you say that you want to simulate the ball joint, do you mean that you want to simulate the kinematic nature of the joint?

One method that quickly came to mind is to represent the shaft (with the ball on it) as a 1-D beam element and use beam releases to capture the nature of the ball joint (all translations are lock and all rotations are free). You can then use weighted links to tie the ends of the beam to relative locations in the model.