Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

stress analysis, find the components that separate into independent components?

11 REPLIES 11
Reply
Message 1 of 12
jasonrecords
3954 Views, 11 Replies

stress analysis, find the components that separate into independent components?

I am running some FEA on an assembly with Inventor 2011. 

I am getting the error that the model separates into 3 independent components.

Is there a way to find which of the parts in the assembly are these 3 components?

At times I have been able to see which these components are by looking at the displacement results (adjusted x5), but this time I am not seeing parts separating?

 

Any help?

 

Jason

11 REPLIES 11
Message 2 of 12
henderh
in reply to: jasonrecords

Hi Jason,

 

  Currently, I'm not aware of any way the user can get a list of the models that "separate".  You can activate the displacement results, and probe on a component.  If there is not a huge displacement, then it is most likely constrained enough.  I've logged a wishlist item to add a way to either list or find the models that "separate" for a future release.

 

  When you see the message about "Model separates into x independent components, weak spring was added" it means that the model has an open degree of freedom. In many cases, this is how a mechanism behaves in real life.  For example, say that you have a pin that is captive, yet it can still rotate...when you use the "sliding / no separation" type contact you will get the separation / weak springs message.  We add the "weak spring" so that we can solve the FEA equations.  Most all FEA packages work similarly in this regard.

 

  I hope this helps!

 

Best regards, -Hugh



Hugh Henderson
QA Engineer (Fusion Simulation)
Message 3 of 12
jasonrecords
in reply to: henderh

Hugh,

 

Thanks.  That does help.  I am using a sliding/no separation on a joint, which is probably as you said is what causing the issue...

Adding to the wish list a listing of what parts are separating would be great!

At least in my example, even using the adjusted displacement of x5, I didn't see any issues.... so I am thinking since I have a joint of a sliding/no separation, my issue is actually a non-issue then.

 

Jason

Message 4 of 12
henderh
in reply to: jasonrecords

Hi Jason,

 

  I think you're right, there is no cause for concern from the message in your case.  I'd like to offer a simpler explanation / scenario, the old "block resting on a table"

 

  1. Create two blocks and mate them together
  2. In Stress Analysis, fix the bottom face of the bottom cube
  3. Create automatic contacts and change the contact to sliding / no separation
  4. Add gravity, in the direction towards the block with the fixed constraint and solve

  You'll see that we get the model separation / weak springs message, but notice that the block doesn't fly off into space, even though it could theoritically spin around or translate horizontally.

 

  Of course in real-life this doesn't happen either, but in FEA equation-land, these are open degrees of freedom and we need to account for these and "lock them out" by automatically adding a "weak spring".

 

Thanks, -Hugh



Hugh Henderson
QA Engineer (Fusion Simulation)
Message 5 of 12
henderh
in reply to: jasonrecords

This topic (and the related 'soft springs' one) keeps coming up from time to time.  The wish list item, to list the components / bodies that separate is 1494847.

 

You may wonder how to get rid of the 'soft springs' message, I'd like to offer a simple example of how to do so:

 

Starting from the beginning, a likely cause is that some components are fully constrained, but certain contact types are allowing movement.  Or there are contacts missing between bodies that need to be created manually (or geometry adjusted so there is no ‘gap’ and automatic contact(s) will be created).  The latter is probably not the case in the most models, since we don’t see the message ‘large deformation, please make sure it’s properly constrained, yada, yada’

 

  We can easily reproduce the ‘soft springs’ condition in a simple assembly of a block resting on a table, or a block resting on another with gravity and a sliding contact:

1.png

2.jpg

 

  Since there is a sliding contact between the top and bottom block, the top block is able to translate from side-to-side (in two directions) and rotate.  In real-life the top block won’t move just resting on a table.  But to FEA, there are open degrees of freedom that needs to be addressed in order to solve the equations.  This is why we must (internally) add soft / weak springs in order to arrive at a result.

 

  The trick to working around these kinds of situations is that you want to be able to lock out the degrees of freedom to not get the soft springs message, but not too much that you would change how the model will be free to deform.

 

  For the resting block example, to lock out the translation in the x and y direction, we can add a fixed constraint to a vertex using vector components.  By saying x and y displacement = 0mm and z remains unchecked, the upper block’s vertex is still free to move up and down:

3.png

  If we simulate now, we’ll still see the weak springs message because there is still an open "rotational" DOF. 

 

  To lock out the remaining DOF, we can add another fixed constraint to another vertex, locking out only the y-direction:

4.png

 

This will keep the block from rotating, yet not over-constrain it and still allow it to move in the x or z direction.

 

Notice that now we no longer get the soft springs message:

5.png

  This is much like constraining components in assemblies.  There are 6 DOF’s open initially, 3 translations and 3 rotations of course.  In most cases, adding one constraint will lock down 3 DOF’s, adding another will lock down two more, the 3rd constraint will lock out the final open DOF.

 

 Another analogy from my fixture design days and GD&T.  In my previous life, I designed fixtures that were used to measure cast parts to ensure they were within the correct tolerance.  Mostly turbine rotors for industrial gas turbines.  They were made in pie-wedge shaped pieces that could be assembled together to make the full-circle of blades, etc.

 

  When you placed one of these ‘wedges’ in the fixture, we don’t want to over-constrain them.  We can accomplish this by touching / resting them at only a point of contact in six different places.  In GD&T there are -A- -B- and –C- datums.  The part is touched in three places with respect to the A datum, two places with respect to the B datum, and finally just one place with respect to the C datum.

 

Hope this helps!

 

Best regards, -Hugh



Hugh Henderson
QA Engineer (Fusion Simulation)
Message 6 of 12
Jeroen_KZM
in reply to: henderh

Hi Hugh,

 

You said   `I've logged a wishlist item to add a way to either list or find the models that "separate" for a future release.`

 

Is there a way to find them?

 

Best regards, Wesley

Message 7 of 12

Can you Attach  your assembly here - I will find them for you.  (And then explain how I found them.)

Message 8 of 12

Hi TheCADwisperer,

 

Do you need a Step? or the complete assambly.

 

In the model there are a few parts that need to be separated. but there is somewhere in model a part that is separated but it has to be bonded. I have looked the model, but can't find it

 

Wesley

Message 9 of 12

A STEP file does not contain any of the information on how you set up your analysis.

Message 10 of 12

Only the .iam is enough? or do you want .ipt to.

because the file is big.

Message 11 of 12
johnsonshiue
in reply to: Jeroen_KZM

Hi! The iam file is not enough. You need to attach all ipt files too. If you want to make the ipt files smaller, you can open each ipt file and move EOP to the top and save.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 12 of 12


@Jeroen_KZM wrote:

Only the .iam is enough? or do you want .ipt to.

because the file is big.


Part FEA is an advanced topic.  Assembly FEA is a step above that. Assembly file structure should be mastered before attempting FEA.

In any case, place all parts and sub-assembly files in a folder along with the top level *.iam file.

Right click on the folder and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file (up to 50 Meg) here.

If it is larger than that you can upload to A360 and provide link.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report