Jump to content
Beginner93

Connect mesh of two components

Recommended Posts

Good evening to everyone,

 

i´ve meshed a Model made out of three components. As you can see, i fixed the nodes between the components with the equivalence funktion. But on one side the components seem not to be fixed the right way. There is only on force in x direction. So the stress in xx in the whole component should be the constant. The analytical result is 40.336 MPa and on two of the three sides it´s right.

image.thumb.png.a5dbdf1e8aae9c77d075ac3eced45544.png

image.thumb.png.380743b44caf52961a53b1cd4bcfc40b.png

 

 

I´ve build the model a few times and get always the same problem. So if anyone could help me, i would be really greatful.

 

Thanks and greetings from Beginner.

Share this post


Link to post
Share on other sites

Hello @Beginner93,

Greetings!!!

 

It would be more helpful, if you could share the mesh picture of your model, with close look near the connection.

 

Also, in edges option, select for find edges - as sometimes, due to low tolerance value provided- set by user, may not equivalence all nodes.

 

If you have free edges(SHift + F3), increase tolerance value and equivalence or manually connect the nodes with replace option (F3).

 

Let us know, if you get desired results from analysis.

image.thumb.png.0e030e45096e73fb0e6091f207ff367b.png

 

 

Thanks & Warm Regards,

Akshay S.Patil

Share this post


Link to post
Share on other sites

Hi,

 

thanks for your hint, but i´ve already tried everything. But always i´ve got the same result. I´ve increased the tolerance up to 0.200 because my mesh size is 0.250. But nothing changed.

 

Maybe there is a problem with the model, but i can´t find anything. If someone can have a short look, i would be very grateful. 

 

Greetings and thanks a lot,

Beginner93

 

 

 

6.38_3_components_Neu_mit_Fx.hm

6.38_3_components_Neu_mit_Fx.h3d

Share this post


Link to post
Share on other sites

@Q.Nguyen-Dai thanks for your help, i know that it couldn´t be the same stress on the whole cross-section with just a single force. But at the beginning and the end of the midsurface-beam i´ve made a slim component with a very high e-module, so the load is distributed on the whole beam. And only the area around x=0 is interesting for me. In this area in the results from two of the three stanchions are pretty good. But in one, as you can see in the picture, is nearly no stress. I don´t know how i can fix this, i tried all the good hints i´ve already got here. Don´t know if i´m just unable or if it isn´t possible the way i´d built the model.

Share this post


Link to post
Share on other sites

Hi,

 

Try creating separate system for your model, make sure X-Co-ordinate is in the loading direction. Change the Resolved in Field to > user system, with the system selector active select the newly created system as shown below. Then check the results.

image.png.1ac4ad0ce94edea9d3008d61c70615a2.png

Thank you

Share this post


Link to post
Share on other sites

@ellison thanks for your help. I already thought the same, so i meshed each surf one by one or meshed all together. But there is allways the same result. I really don´t know where is the problem. Is it the mesh or the model or anything else, i really don´t know....

 

Thank you

Share this post


Link to post
Share on other sites
On 5/11/2018 at 11:41 AM, Premanand Suryavanshi said:

Hi,

 

Try creating separate system for your model, make sure X-Co-ordinate is in the loading direction. Change the Resolved in Field to > user system, with the system selector active select the newly created system as shown below. Then check the results.

image.png.1ac4ad0ce94edea9d3008d61c70615a2.png

Thank you

@Beginner93, try this. It works.

 

Thank you

Share this post


Link to post
Share on other sites

Hello,

 

Premanand Suryavanshi is right with his help, here is a short explanation.

 

If you are plotting X-component stresses in analysis system, then the stresses are orientated on the local element coordinate system.

The X- direction of the top plate doesn't show all in the same direction. You can check it with Hypermesh->Tools->Orientation Review. See attached picture.

 

You can either reorient the elements, or use the proposed tensor transformation by the "Resolved in:" shown in upper picture.

You can take global direction, or define a user system, or define projection rules.

 

Best Regards,

Mario

 

 

image.thumb.png.356c5a6e1d3e644b772e00717076d818.png

 

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...