Geometry Error

[Juanjaviertorresgoitia]

I am trying to perform a Finite Element analysis of a 120 in. aluminum extrusion which is a subpart of a curtain wall system. This extrusion plays the role of the mullion on the system and is subject to wind loads. The model contains three different materials: Aluminum, rigid PVC filler and a polyethylene thermal barrier break.  I was performing the analysis on Autodesk Mechanical and I receive a “Geometry Error” window message that reads: “The model contains errors due to geometry problems. Do you want to view these errors?” I have attached a copy of the note pad file generated that lists these errors. How can I fix this geometry problem?  Or at least narrow down on the model to know where the issue stems from?

Thank you

[AstroJohnPE]

Javier,

The message says that the geometry decoder did not find any 1D elements. This implies that one of the parts is defined as truss or beam elements but the mesh does not represent those element types.

• Is that possible?
• What are the element types for all of the parts?
• Which parts came from a CAD model?
• What type of constraints do you have on the model?

The other possibility could be the path where the model is stored although I think it is shorter than the allowable limit, and hopefully the parantheses ( ) and comma , are not part of the problem.

[Juanjaviertorresgoitia]

John,

Tthanks for your feedback. I did define all the 8 the components of my model as beams. I started with 2D ".dwg"'s in AutoCAD (one file for each of the 8 components of my model), which then I imported to Autodesk Inventor where I created the extrusions. On Inventor, opening a "Standard.ipt" file and then under the "Sketch" tab in the "Insert" menu I imported each of my 8 components “.dwg”  files and created the 120 in. extrusions. Having extruded all 8 parts and saved them independently as ".ipt"’s I assembled them together opening a "Standard.iam" file. Once the blank file opened, under the "Assemble" tab in the "Place" menu I placed each of the 8 ".ipt" extrusions. It is here that I assigned the "Place Constraints" for each part (flushed at each end and no sliding between them) using the "Constrain" option on the "Position" menu under the "Assemble" tab. Once all the constraints were set I used the "Start Simulation" under the “Add-Ins" tab, which exported my model from Inventor to Simulation Mechanical. Once on Simulation, I created a solid mesh using the “3D Mesh Settings” menu under the “Mesh” tab with an absolute mesh size of 0.25 in and with 7 retries with a reduction factor of 0.75 (I clicked on the "Generate 2nd order elements" box). Once the model was meshed I assigned the material properties to each of the 8 components (5 Aluminum (6063 T6), 2 Polyurethanes and 1 Rigid PVC, for the Polyurethane and PVC the properties were added manually to the material library). Then under the "FEA Editor" tab on the left side of the screen under the "Parts" collapsible menu each Part's "Element Type" was manually changed to "<Beam>" from the default "<Brick>" elements. On the same menu for each "Part", under the "Element Definition" option I manually inputted the part's properties (Area, moments of inertia (x&y), polar moments of inertia and section modulus). Finally, the reason that I needed the "Element Type" to be beam elements is because I needed to apply wind loads to some surfaces off the model (in units of lb/in). The only way I could find an option to apply a distributed load that would approximate a wind load scenario was applying a distributed load which Simulation only allows to be applied to beam elements. When I run the analysis is where the "Geometry Error” pops up.

I will get rid of the “()” and comas and give it a try

This is a long explanation…., but hopefully you can get an idea of what I’m doing and point out what might be causing the issue   

Again thanks for your time!

[AstroJohnPE]

Hi,

A beam element is a line drawn along the length of a "beam" at the centroid. So the mesh does not represent the volume of the model; the cross sectional properties that are entered in the Element Definition define the volume of the model. A beam model looks like a stick figure. Please see Figures 1 and 2 on the page "Design Optimization of Beam Elements" in the documentation to get a better understanding.

Since your element type (beam) is wrong for the type of mesh you created (3D solid), I can think of two options:

(1) redraw the model as lines (a stick figure) and analyze it with beam elements. For long slender structures, this is a good approach.

(2) keep your solid model and 3D mesh and change the element type to brick. The cross section of the solid parts represent the cross section of the "beams". The wind load can be applied as a pressure because you know the distributed load (load per length) and you know the width where the load is applied (width). Pressure = (load per length) / (width). If the load varies over the length, you can use the "Setup > Loads > Variable Pressure" command to write a formula for the pressure as a function of the length.

[Juanjaviertorresgoitia]

John, it has been a while. I wanted to get maximum moment stresses from the results of this wind loaded aluminum mullion FEM that we were discussing. I ended up modeling it as a brick element type system to better approximate a wind load condition, following your suggestion (option # 2 on the last correspondence) and I was able to run the analysis. However, Autodesk Simulation Mechanical only provided me the resulting stresses as von Mises stress (in units of lbf/in^2) which makes sense having modeled the mullion with brick type elements. I was wondering if there is a way of getting the resulting moment stresses of the mullion as regular beam moments, the ones you would get applying beam formulas. Let me know if I need to clarify 

Thanks again! 

Javier    

[AstroJohnPE]

Hello Javier,

Please look at the thread Extracting Forces and Moments. That dicussion gave a method, and I just posted a "test case" to the thread. See if it works for your situation.