MESH SPIRAL DUCT

[zsolti_sdd]

Hy everyone

for my master degree i need some help,

to mesh a spiral duct in Nastran , from attachment. ( in the picture the real compression from lab.)

it is for an axial compression.

I tried several times to mesh but error every time.

Drawing model : Inventor 2018

REAL material : Z150 DX51D , but i didn't find it in nastran, and i use steel1025.

thank you

[John_Holtz · Accepted solution]

Hi @zsolti_sdd

I tried to mesh the JPG file, but I could not get it to mesh either. In other words, you need to provide the Inventor file so that someone can look at the model to determine the problem.

But before you do that, I suggest that you create a surface model in Inventor (instead of a solid model) so that you can generate shell elements in In-CAD. Your material is very thin, so solid elements will not give accurate results because 1 element through the thickness does not calculate bending/moments. Shell elements do calculate bending/moments, and the shell model will probably mesh okay.

For future reference, this article gives some tips on what to do when a solid model fails to mesh: Meshing Failed when solid meshing with Nastran In-CAD. There are many reasons why different models fail to mesh, which is why the article also links to Nastran In-CAD: How to resolve meshing issues.

[zsolti_sdd]

helo

[John_Holtz]

Hi @zsolti_sdd

I did not try to mesh your model because I am sure that it is wrong. Because there is no gap between the faces, the joints have become one big blob of material instead of 4 overlapping thicknesses. This is not want you want to have for your analysis.

Section view. Need a gap between faces

I was not able to adjust your sketch; I could not understand where some of the geometry was dimensioned, so I could not change the dimensions. Essentially, you want to put a small gap, such as 0.1 or 0.2 mm between the joints so that it will look something like this.

with gap between faces

The gap in the model can be "removed" in the analysis by using a "penetration offset distance" on the contact definition.

[zsolti_sdd]

Helo

Thanks for your response.

somebody helped me to draw the spiral air duct. I don't know the Inventor 3d. 

My topic : https://forums.autodesk.com/t5/inventor-forum/spiro-ventilation-duct/m-p/7813564#M684311

in reality looks like this (see atachement) and i can not  measuring the gap. 

have a nice day

[John_Holtz]

Hi @zsolti_sdd

I see another problem in the Inventor file. There is in interference where the parts interlock. The interference is at the green arrow in the image below. (I merged two images from the sketch and color-coded the two ends of the same sketch red and blue.)

What you want to create is shown in the bottom half of the above image. The black arrows show the 4 locations where you need a gap so that the solid model does not "melt" together.

Whether you make the solid model in Inventor or some other program does not matter because you can always open or import it into Inventor. (If you can figure out FEA, I am sure that you can figure out how to create the model in Inventor .) In fact, the entire sketch of the cross-section can be worked out from the 5 dimensions that I have highlighted in the attached "sample sketch". All of the other dimensions are linked (shown by the dimensions "fx:") to a combination of those highlighted dimensions. For example, the diameter of circle 2 = thickness of material+2*gap. (If using Inventor, I suggest that you start the sketch by drawing the 4 circles that I have indicated, and then drawing lines off of those to complete the sketch.)

Regarding the gap, you do not need to measure it on the physical part. You just need to create one in the solid model so that the "hooks" are separate when you sweep the sketch around ("Coil" command in your sample Inventor model). Whether you make the gap 0.01 or 1 does not matter because you will use that same dimension to offset the contact surface in the analysis to eliminate the gap. (1 may be too large depending on the thickness of the material, but at least mathematically you can use any dimension. Considering the accuracy of the analysis, the dimension of the gap is the least of your worries.)

Have fun!

[zsolti_sdd]

hello

I tried several times to mesh but failed.

I changed the sweeped section, followed the instructions with gaps.

have a nice day

[John_Holtz · Accepted solution]

Hi @zsolti_sdd

A mesh size of 20 mm worked. That is still a bit coarse, so you may ultimately want to use a smaller mesh size. (What I normally do in these types of cases where a solid does not mesh is to delete the solid idealization and create a shell idealization with a triangular surface mesh. That worked with the 49 mm mesh size but looked very coarse. That's when I tried the 20 mm mesh size and then tried the 20 mm mesh size with a solid idealization.)

Have you given any thought to using shell elements?

[zsolti_sdd]

HELO

Thank you very much, its working.

how can i load the surface axial force to  go all the way down (the bottom) of the airduct.

Exist any method to export all the measuring results in PDF or Power point, like the Autodesk Moldflow.?

thank you once again

have a nice day

[John_Holtz · Accepted solution]

Hi @zsolti_sdd

I am not clear what you mean by your question "how can i load the surface axial force to  go all the way down".

1. If your question is how to apply the load over the entire face, you should be able to select the faces to which you want to apply the load. (Of course, you can select other types of geometry to apply the loads, such as edges, as needed.)
2. If your question is how to get the displaced shape to look like 2340 mm (according to the legend, or 936 mm that is shown by the max probe), you need to edit the plot and change the deformed scale from "Percent" to "Actual" with a value of 1. In other words, I think the amount of deformation shown is only a fraction of what the displacement value is.
3. If you question is how to crush the duct completely (like stepping on a soda can), you will not be able to do that. The elements would need to distort too severely to do that, and there is a 99.9% chance that the analysis will not converge. You should be able to get to the point where it starts to buckle. You need to perform a nonlinear transient analysis or nonlinear buckling analysis. It looks like you are performing a linear static analysis.

[zsolti_sdd]

helo

thank you for the solution.

I accept the second solution.

Reffering to the 3rd solution, YES, i want to be crushing like a soda can, but it very complicated to me, to do the necesary settings(mesh, shells, idealization, creat material....) for the circular airduct  axial compresion  in Nastran.

have a nice day

[martin_madaj]

Regarding the point #3 of John Holtz's answer, you might want to try to activate the Arc-length method in a nonlinear solution setup. But definitely it will need some parameter tuning to get it work.

Best regards,
Martin Madaj.