Structural-Thermal analysis error : element type

  • 166 Views
  • Last Post 21 May 2019
Zenia posted this 18 May 2019

 

sorry for my poor english. I'm total beginner in this field so I need your help.

I have a rotating shaft with a gear.

My goal is to analyze how much friction heat is generated from the rotation with frictional contact.

Used codes are the followings :

 

- geometry, for bodies (rod, gear) :

   et,matid,226,11 (gear)

   et,matid,226,11 (rod)

 

- frictional contact with coefficient 0.4 : 

   keyopt,cid,1,1

   rmodif,cid,15,1

   rmodif,cid,18,0.5

 

- named selection(all bodies) as 'them' : 

   sf,them,conv,680,22

   allsel,all

 

and as i press the solve button i got this error:

 Element type 1 is not the same shape as SOLID226.  Switching to a      
 different shape is not allowed while elements of type 1 exist.   

 

how to solve this error?

i referred this vid.  

Attached Files

Order By: Standard | Newest | Votes
jj77 posted this 18 May 2019

This is not a beginner analysis - make sure you take first a course on basic FEA before you undertake this type of analysis.

(e.g., https://onlinelearning.cornell.edu/hands-introduction-engineering-simulations-mooc)

 

Another thing once you get the basic is to read through the messages you get from a solver.

 

So here it says element type is not the same shape as solid226 (see that element for more info). So it is because this hexahedral element is assigned to TETrahedral elements. 

 

So you need to address that have all solid227 thus all tetrahedral meshed, since your parts can not be meshed with only hexahedrals  (so both commands should be).

et,matid,227,11

 

You might also need to add Cv and Enthalpy in mat. properties for steel

 

 

  • Liked by
  • peteroznewman
  • Zenia
Zenia posted this 19 May 2019

Thank you for your answer.

I changed the code as following :

et,matid,227,11 ( rod, gear )

or

et,matid,227,11

et,matid,226,11

( rod, gear )

 

but both code makes same error : 

 Element type 1 is not the same shape as SOLID227.  Switching to a       
 different shape is not allowed while elements of type 1 exist.   

 

one notable result was the mesh of the shaft became pretty homogeneous.

how to add Cv(constraint variable?) and enthalpy?

 

p.s.: i watched the course but there wasn't such type of vid(coupled field analysis)

peteroznewman posted this 19 May 2019

Using SOLID226 on the disk and SOLID227 on the rod takes care of the shape of the target element matching the shape of the elements in the mesh, since the disk has a tetrahedral mesh and the rod has a hex mesh.  There are mesh controls you could use to force that to happen, it is currently happening by default, but if you change the geometry of the rod, it could mesh with tet elements next time.

You also have to match the order of the target element with the order of the elements in the mesh.  SOLID227 is a quadratic element.  To force the mesh to create quadratic elements, on the Mesh Details window find the Element Order setting. Change it to Quadratic.

Then you get this error:

 *** ERROR ***       CP =       1.031   TIME= 17:12:56
 The calculated specific heat at constant strain (Cv) is negative.  (See section "Thermoelasticity" of the Theory Reference for the definition of Cv.)
Please verify the input of thermal material quantities for consistency.

Try defining Cv in the Engineering Data for the material you use (as jj77 suggested).  I did that but it didn't fix the error. AnPham might have a suggestion for getting this model to run, he provides his email address in the discussion below.

Here is one relevant discussion.

Here is another relevant discussion.

  • Liked by
  • Zenia
Zenia posted this 20 May 2019

Thank you for your kindness, peteroznewman.

I changed my setting as you say : 

et,matid,227,11(rod)

et,matid,226,11(disk)

element order : Quadratic

 

it still makes the same error : 

 Element type 1 is not the same shape as SOLID227.  Switching to a      
 different shape is not allowed while elements of type 1 exist.      

 

I can't find the way how you solved this problem.

Once I solve this problem then I can get to the next level problem such as Cv(contraint strain?) and so on.

peteroznewman posted this 20 May 2019

What version of ANSYS are you using?

  • Liked by
  • Zenia
Zenia posted this 20 May 2019

My ANSYS version is 18.2.

I never thought it woulb be difficult that much.

I'm keenly someone's help.

peteroznewman posted this 20 May 2019

As jj77 says, this is not a beginner analysis.

Attached is an ANSYS 18.2 project archive. You must use File > Restore Archive to open it.

This has the Cv error.

Attached Files

  • Liked by
  • jj77
  • Zenia
Zenia posted this 20 May 2019

Oh Jesus Thank you so much

I can't find yet any difference between mine and yours, but it at least doesn't make type error.

You saved me really thank you.

It still makes Cv error as you said but now I'm free from type error!!

jj77 posted this 20 May 2019

The difference is that rod should be 226 (HEX - 20 nodes) and disk/gear, 227 (TET - 10 nodes) - hope this helps to clarify

  • Liked by
  • Zenia
  • peteroznewman
Zenia posted this 20 May 2019

Thank you so much jj77 and peteroznewman. I could get so far here thanks to you.

strange one is that there is no difference between his and mine.

now there only remains Cv error.

I know nothing about this but I guess it is related to the engineering data.

jj77 posted this 20 May 2019

Yap, also check your model dimensions and units (use SI units every where). The disk is 90 m wide .

 

As for the Cv if we insert this then it works (in command snippet for solid226 and 227 conversion):

Have in mind this is just an example, so they need to be changed to the values specific for your material

 

Add these to both apdl command snippets:

MP,EX,matid,200E9 ! E mod.

MP,NUXY,matid,0.3 ! Poisson's

MP,DENS,matid,7800

MP,CVH,matid,448 ! Or this works some times (Cp): Use this instead then MP,C,matid,448

MP,ALPX,matid,0.000012

MP,KXX,matid,0.0001

 

Now I am not sure exactly why it does not work when Cp is entered )could be related to the very large dimensions, because I have not found how ansys calculates Cv. Edit: It does  work now when it is changed back to Cp - not sure why

 

  • Liked by
  • peteroznewman
Zenia posted this 20 May 2019

Thank you jj77. I will never forget this.

Cv error suddenly gone as I change to the original geometry - the gear with the shaft.(also original unit )

now the only problem is the following : 

-----------------------------------------------------------

Element 89 located in Body "rod" (and maybe other elements) has become highly distorted.  You may select the offending object and/or geometry via RMB on this warning in the Messages window.  Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere.  Try incrementing the load more slowly (increase the number of substeps or decrease the time step size).  You may need to improve your mesh to obtain elements with better aspect ratios.  Also consider the behavior of materials, contact pairs, and/or constraint equations.  If this message appears in the first iteration of first substep, be sure to perform element shape checking. Named Selections for the offending element can be created via the Identify Element Violations property on the Solution Information Object.

----------------------------------------------------------

I will attach the newest file with the error.

I hope this is the last gate to the next level. thank you masters.

Attached Files

jj77 posted this 20 May 2019

I have never done something like this and I can imagine it needs a lot of twicking to get it work, and I would not how to do it, since i do not have experience in this type of simulations (because as I said engineers which I help and teach never do this, they are structural engineers), so I cannot help you

Zenia posted this 20 May 2019

OK I see...  

But I will never forget your kindness which brought me here.

I will do my best to solve the remaining problems.

If were not you, I wouldn't have started this, just giving up.

Regards.

jj77 posted this 20 May 2019

All the best.

 

Perhaps AnPham might have some advice, since he seems to have dome some models like yours

 

peteroznewman posted this 20 May 2019

1) The disk is still about 25 meters across. As jj77 suggested, that can't be correct.

2) While you are in the geometry editor, divide the face of the rod at the top and bottom planes of the disk, and update the Contact to pick just that part of the rod.

3) Delete the Rotational Acceleration of 15 rad/s^2. This causes ALL bodies to have a rotational acceleration.

4) Create a Joint Load on the Revolute Joint of Rotational Acceleration of 15 rad/s^2. This causes the disk to spin on the rod.

5) Check the Initial Contact Status with a Contact Tool under the Connections folder.  If the contact is open, no heat will be generated. You can apply an offset in the Contact definition to create some interference.

 6) Use a finer mesh.

Zenia posted this 21 May 2019

Appreciate for your answer.

I did as your words , which are correct size(cm unit) and the finer mesh and it still makes the error.....

I got highly distorted error and negative Cv error...

I attached the newest file and watch them and give me some advice please.

Currently, I have not enough time to finish even a single project.

So if no one can help me, then I will consider to change the topic of my project.

Regards.

Attached Files

peteroznewman posted this 21 May 2019

The face of the rod has not been divided into 3 faces.

The mesh is still too coarse.

This is not a good project for a beginner in ANSYS.

I am on a few weeks vacation starting tomorrow.

  • Liked by
  • Zenia
Zenia posted this 21 May 2019

Thank you for your answer. Maybe It's time to accept my level. This is not a easy stuff for me. I couldn't solve problems even though I got so many help from you. I need to find another topic which is easier than this and worth it. And I need to pursuade my team to change the topic as soon as possible.

I really thank you for every word you've done.

Close