Cancel
Showing results for 
Search instead for 
Did you mean: 

Failed mesh -- how to find element ID?

PLM World Member Legend PLM World Member Legend
PLM World Member Legend
I am trying to run an analysis and it returns a fatal error saying the mesh quality needs improving. Element 44761 fails with an aspect ratio of 100.11 (tolerance = 100). How do I locate where element 44761 is so I can get an insight into what to change in the 3D model? In general, how do you locate an element if you know the ID number?
8 REPLIES

Re: Failed mesh -- how to find element ID?

Siemens Phenom Siemens Phenom
Siemens Phenom
From the FEMAP menu - Window - Show Entities, change the selection to Element, hit ok, and then type in Element 44761 and then hit ok in the selection box and FEMAP will highlight the element you entered. From the Custom Tools Toolbar button, you can also jump down to "Meshing" and in "Meshing", there is an API that I wrote the highlights the worst element in the model, and also centers the view on that element so you can quickly zoom and and take a look at it.

With the FEMAP v10.3 that you're using, we added a Mesh - Geometry Preparation tool that might be able to clean up geometry slivers and such so that you don't have to do these things manually. Delete the mesh that you have now, and run Mesh - Geometry Preparation before meshing, this should fix things up. If you get stuck, e-mail me the geometry - sherman.mark@siemens.com and I can steer you to the best path for getting a good mesh.

Mark Sherman
FEMAP Development

Re: Failed mesh -- how to find element ID?

PLM World Member Legend PLM World Member Legend
PLM World Member Legend
Thanks for that! The only problem with the show entities is that the element highlights for a fraction of a second only then disappears! How do you get it to stay highlighted long enough to be studied? Likewise, with the API the view centres to the worst element but does not highlight it.

I am now playing around with the geometry prep tool and that seems to make a difference.

Thanks for your time! If you can clarify how to keep an element highligted that would be great.

Re: Failed mesh -- how to find element ID?

Community Manager Community Manager
Community Manager
Take a look at this Femap Tip and Trick video, it shows you how to find and view the worst elements in the model:

http://www.youtube.com/watch?v=3joCI8lYOQo

Al Robertson
Siemens PLM

Re: Failed mesh -- how to find element ID?

Community Manager Community Manager
Community Manager
Take a look at this Femap Tip and Trick video, it shows you how to find and view the worst elements in the model:

http://www.youtube.com/watch?v=3joCI8lYOQo

Al Robertson
Femap Marketing

Re: Failed mesh -- how to find element ID?

PLM World Member Legend PLM World Member Legend
PLM World Member Legend
Hi Al,

Thanks for that. Unfortunately access to youtube is blocked at our site. Is there any other way to make that video available?

Cheers,

Chris

Re: Failed mesh -- how to find element ID?

Community Manager Community Manager
Community Manager
Hi Chris,

Yes, you can also see it on the Siemens PLM Femap demos page:
www.siemens.com/plm/femapdemos

Femap tips and tricks are on the right, and Element Visual Inspection is the at the top of the list.

Regards,
Al Robertson
Femap Marketing

Re: Failed mesh -- how to find element ID?

PLM World Member Legend PLM World Member Legend
PLM World Member Legend
Hi Al,

Thanks for that!

Chris

Re: Failed mesh -- how to find element ID?

Solution Partner Valued Contributor Solution Partner Valued Contributor
Solution Partner Valued Contributor
If you get any elements like that, it is almost always a by-product of very large ratios of adjacent geometry features in the model, or the use of a large element size together with small geometric features. Eg. if there is a curve or surface in the model which is 2mm, adjacent to a much larger entity, and your mesh size is 100mm. The geometry preparation method is a good choice, because it quite nicely identifies these types of issues and attempts to combine small feature curves / surfaces into larger adjacent ones, so the meshing is not attempting to define features which are not significant to the engineering. Using a smaller mesh size can often cure mesh quality problems as well, but I know that has limits, and I think the download version is only 32 bit (could be slow if the model is "large").

If there are still problem elements and you want a persistent method to see them properly, there are two good methods:


1. Group | Create/Manage -> New Group
Group | Element ID (and enter the ids)

This creates a new group, and tells Femap which element(s) are in it (and there are nice ways to get info from the run-files and paste it into the entity selection box)
Then down in the bottom right hand side of the Femap window click on "Grp" and choose "View Active" which displays only the Active Group.

2. Tools | Check | Element Quality. You can choose what checks to use (eg aspect ratio, and set the threshold), and then choose the option to create a group of the distorted elements. Femap will automatically create the Group, then you can use the Grp button in the bottom right of the Femap window (as above) to view only the active group.

However, as mentioned first, elements of 100:1 aspect ratio (which cause the analysis to fail) are primarily a by-product of the ratio of element size to small geometry detail. If that is addressed, the problem goes away.