## Simulation Mechanical and Multiphysics

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic to the Top
- Bookmark
- Subscribe
- Printer Friendly Page

# Plate Element Results - Confused by 2014

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Hello Everyone,

I am getting some results that I find rather confusing. I am getting more results than I expected from the same node. I have plate elements in everthing here. I highlighted the nodes of the same part. The thickness of the refered part is 1" (25.4mm). I am running 2014 with SP1 of the Adesk Mechanical Simulation software.

My question is basically why am I getting 4 results at one node and only two at the other? Herebelow you may find the inquire results dialog from those two nodes.

NODE WITH 4 RESULTS

___________________________________

Current Load Case = 1

Node # 23728 ( X = 116.668, Y = 198.002, Z = -116.059 )

Displaced Position : X = 116.584, Y = 198.274, Z = -116.051

Displacement = DX: -0.0845752, DY: 0.271747, DZ: 0.00808071, Magnitude: 0.284719

appears in 4 Element(s)

Part: 2 Element: 421 (top)

Part: 2 Element: 506 (top)

Part: 2 Element: 507 (top)

Current Result Value: 24.57620172 N/(mm^2)

Part: 2 Element: 420 (bottom)

Current Result Value: 28.68452725 N/(mm^2)

Part: 2 Element: 420 (top)

Current Result Value: 31.33315928 N/(mm^2)

Part: 2 Element: 421 (bottom)

Part: 2 Element: 506 (bottom)

Part: 2 Element: 507 (bottom)

Current Result Value: 35.75895312 N/(mm^2)

NODE WITH 2 RESULTS

___________________________________

Current Load Case = 1

Node # 23576 ( X = 19.004, Y = 164.991, Z = -18.9048 )

Displaced Position : X = 18.9246, Y = 165.28, Z = -18.8979

Displacement = DX: -0.0794382, DY: 0.288677, DZ: 0.00687432, Magnitude: 0.299487

appears in 4 Element(s)

Part: 2 Element: 169 (top)

Part: 2 Element: 170 (top)

Part: 2 Element: 297 (top)

Part: 2 Element: 298 (top)

Current Result Value: 15.88908161 N/(mm^2)

Part: 2 Element: 169 (bottom)

Part: 2 Element: 170 (bottom)

Part: 2 Element: 297 (bottom)

Part: 2 Element: 298 (bottom)

Current Result Value: 16.52662907 N/(mm^2)

Please note as well that the colours are not so smooth.

What is hapenning? This kind of model used to work in version 2013 of the software.

I greatly appreciate the help

Solved! Go to Solution.

# Re: Plate Element Results - Confused by 2014

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

I tried refining the mesh but the results are the same.

# Re: Plate Element Results - Confused by 2014

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Well, the two results are because plate elements have different results on the "top" versus on the "bottom".

This is just a guess from trying to interpret the "Inquire Results" dialog, but it appears that the top side of elements 421, 507, and 507 is facing you but the bottom side of element 420 is facing you. So it reports the average stress on the top from 3 elements, the stress on the top from one element, the average stress on the bottom from 3 elements, and the stress on the bottom for one element.

I cannot tell from the images, but my guess is that the plate lies in a plane that passes through the origin (0,0,0). This coordinate is the default "Element Normal" coordinate entered in the Element Definition. Due to round-off, or just by the way the face is curved, most of the elements were created with the normal direction pointed in one direction, and the other few elements (the ones that do not look to be smooth) have the normal direction pointed in the opposite direction.

BTW, the normal coordinate and direction determines which side is top and which is bottom. "Resuls Options > Element Orientation > Element Axis 3" will show the normal direction for every element.

Mechanical Engineer

Pittsburgh, PA

Simulation Mechanical user since Dec 1997

# Re: Plate Element Results - Confused by 2014

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Hello AstroJohn,

You are the best. As you said, the thing is somehow the orientation of the elements got all messed up.

You have already helped me several times and I deeply thank you for that.

Anyway, why did this happen?

The characteristics of this model are a bit complicated because the plate is not perpendicular to the profile. It is slightly tilted (2 degrees). Not only that, but it is also inclined about 45 degrees in refererence to the profile axis.

**How can I solve this? More importantly - are these results trustworthy?**

# Re: Plate Element Results - Confused by 2014

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

You can solve it by

- Edit the Element Definition for the parts made of plate elements.
- Enter a coordinate for the Element Normal that does not lie in the plane of any element.
- If you do not have any pressure or temperature load on the plate, the direction of axis 3 usually does not matter. Having a consistent direction for axis 3 seems to be the important item.

Mechanical Engineer

Pittsburgh, PA

Simulation Mechanical user since Dec 1997

# Re: Plate Element Results - Confused by 2014

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

That did the trick.