## Questions about a finite element modeling situation ?

## Questions about a finite element modeling situation ?

(OP)

Hello everyone,

I am currently modelling a part with finite elements in Patran, and I have encountered a small problem. Basically I have a part that is made out of several hollow beams and solid plates, and I have modeled everything with shell elements. The problem occurs at 4 beams that run through the whole part, these beams have a square hollow variable section (it starts at 14 mm edge length and ends at 10 mm). All the beams in the part were modeled with shell elements constructed at the mid-surface of the section, except for these 4 beams for which the elements where constructed on the exterior surface (I had to use the exterior surface because of the way the part was designed, it was easier to model this way).

Now I have 2 questions regarding my FE model:

1. As you can see on the picture I have attached, when I input the shell properties I use a shell offset for the thickness, this generates a material overlap which basically increases my overall mass. Because the thickness is quite high (3mm) and there are 4 beams I get a difference between the mass of my FE model and the mass of the CAD model of 170 grams (CAD Model: 2800 g and FEM Model: 2970), an error of 6%. How can I reduce this difference ? (without changing the FEM model)

2. Is this material overlap increasing the stiffness of the model ? will this have a very big impact on the overall strength and give wrong results ?

Thank you very much,

Cosmin

PS: Sorry for my English, I am not a native.

I am currently modelling a part with finite elements in Patran, and I have encountered a small problem. Basically I have a part that is made out of several hollow beams and solid plates, and I have modeled everything with shell elements. The problem occurs at 4 beams that run through the whole part, these beams have a square hollow variable section (it starts at 14 mm edge length and ends at 10 mm). All the beams in the part were modeled with shell elements constructed at the mid-surface of the section, except for these 4 beams for which the elements where constructed on the exterior surface (I had to use the exterior surface because of the way the part was designed, it was easier to model this way).

Now I have 2 questions regarding my FE model:

1. As you can see on the picture I have attached, when I input the shell properties I use a shell offset for the thickness, this generates a material overlap which basically increases my overall mass. Because the thickness is quite high (3mm) and there are 4 beams I get a difference between the mass of my FE model and the mass of the CAD model of 170 grams (CAD Model: 2800 g and FEM Model: 2970), an error of 6%. How can I reduce this difference ? (without changing the FEM model)

2. Is this material overlap increasing the stiffness of the model ? will this have a very big impact on the overall strength and give wrong results ?

Thank you very much,

Cosmin

PS: Sorry for my English, I am not a native.

## RE: Questions about a finite element modeling situation ?

2) you are modelling all these shells, ie as you show in the overlap. why not delete one set within the overlap ? how is the box beam ass'y made ? are pieces welded together ? (then you can model that way)

another day in paradise, or is paradise one day closer ?

## RE: Questions about a finite element modeling situation ?

2) The shells can't be deleted because they will intersect other beams or plates. This part is quite complex, so complex that it can't be realized by traditional manufacturing, we will 3D Print the part using AlSi10Mg metallic powder.

I talked with some fellow stress engineers and they have suggested that I could locally modify the density of the material in the overlapping zones. Is this a good practice regarding FE modelling ?

## RE: Questions about a finite element modeling situation ?

2) As I understand it you have overlapping shells. These overlapping areas either have the same mesh, or could be modified to have the same mesh. I can't see why you can't remove one of the duplicates.

changing density would improve the weight estimate of the model (if that is that important to you).

a thought ... why not TET mesh (use 3D TET10 elements) the CAD model part ? Then you model would be exactly the same as your part.

another day in paradise, or is paradise one day closer ?

## RE: Questions about a finite element modeling situation ?

2) No, the shells are not overlapping. What I was trying to say is that when I input the thickness with offset to the plate, I will basically have "double" the material in the overlapping zone because the shells are at the outer surface and the offset is directed inwards.

Originally the plan was to use solid elements (because of the complexity of the part) but we are running a random vibration analysis and it wont run with more than 20,000 solid elements (at least the license that we have doesn't allow this). Right now, by using a coarser mesh, the model has approximately 50,000 shell elements so it's impossible to go below 20k tet elements.

## RE: Questions about a finite element modeling situation ?

Depending on what results you're after, the stiffness (and stress) may be very different if you use exterior surface instead of the mid-surface. Let's say your thickness is 3mm, let's also say at a particular cross section of your beam, the mid-surface model width is 12mm and the exterior surface width model is 15mm. The tensile area per side is respectively 36mm^2 and 45mm^2 (25% difference). The area moment of inertia difference between the two cases would be much larger.

I agree with

rb1957where a solid model is the way to go if the shell approximation doesn't fit your requirements. You could try CMS to get around the element count limitation.Best regards,

Sze Kwan (Jason) Cheah

## RE: Questions about a finite element modeling situation ?

2) I don't understand. your pic shows an overlap. the talk has been about shell elements. So I assume the pic shows shell elements overlapping.

3) maybe you can get a one-time license ?

hi jason !

another day in paradise, or is paradise one day closer ?

## RE: Questions about a finite element modeling situation ?

Ionut Cosmin1)Your seniors rightly pointed to change the density of the model for the extra material you are putting. This will take care of mass part of your vibration analysis. But see if you could be able to find verified solution w.r.t. any similar past project or analytical solution if available. Then you can compare the result and get even.

2)The stiffness part is also important. The extra material you put will surely increase the stiffness and hence the stress and frequency results will differ. How much wrong? Compare the analytical/past project/reference paper results if available.

One way I see is to model solid and shell together where solid for complex part and shell for simple part assuming you have overall limitation of 20k elements on solids only.

## RE: Questions about a finite element modeling situation ?

I think this is an acceptable practice, the results will for sure be much more correct than with no density and modulus reductions.

prex

http://www.xcalcs.com : Online engineering calculations

https://www.megamag.it : Magnetic brakes and launchers for fun rides

https://www.levitans.com : Air bearing pads

## RE: Questions about a finite element modeling situation ?

JasonI have already used the exterior surface for these beams, and it will be time consuming to modify everything. I can't use CMS because it is forbidden by the FEM Requirements of the project.

rb19571) well this part will need to be manufactured and send to space and we have a strict deadline so as to not miss the launch date of the rocket :))

2) No, the shells are constructed on the exterior surface of the beams and when I plot the thickness of the shell you will get an overlap in the corners (I"ve attached a picture to better understand, although in the picture the shell are at mid-surface)

3) not enough time right now

NRP99Unfortunately I don't have any projects results for a case like this. Initially I have made a model with solid elements and shell elements with RSSCON connections but the design was changed pretty much and I went only with shell elements because it was simpler to do.

prexThis is what I am going to do, it seems to be the best solution at the time.

Thank you all for your answers, I really appreciate it !

## RE: Questions about a finite element modeling situation ?

I've added a little red square to show the overlap, and a little blue square for missing material, right?

So you have elements finely meshed in the corners ? (like t/2, to capture the overlap)

another day in paradise, or is paradise one day closer ?

## RE: Questions about a finite element modeling situation ?

rb1957Yes the red is the zone with the overlap. Yes the elements are finely meshed on the corners

## RE: Questions about a finite element modeling situation ?

prexCan you please explain your following point for better understanding?

I get the point of decreasing density to decrease the mass and also reducing the modulus for reducing the the stiffness for the extra material considered. But why divide it by 2? Why not some random number? Is there any guideline for situations like this?

## RE: Questions about a finite element modeling situation ?

I have run a modal analysis (SOL103) on the elements with the default properties and then other 3 simulations, on the shell_out model, modifying the density and elasticity modulus on the elements from the corner, as seen here

The results are centralized here. Results show that the outer model adds some stiffness to the model and even while decreasing E by half, the stiffness remains high. It seems that only by decreasing E a lot (something like 80%), I would reach the same results as the solid and shell_mid model. Also the density had to be reduced by 40% on the corner zones to reach the same mass between the models.

## RE: Questions about a finite element modeling situation ?

Ionut CosminAt corners you don't have material. So ideally the stiffness should be zero which is why you get stresses close when you reduce the E to 80% compared to solid model. Check whether you get results as close as possible by reducing E to 80-99%.

Density reduction will depend on the amount of mass to be reduced. We generally calculate it by taking ratio of mass vs density.

I am waiting for the reply of the my earlier question. Anybody have pointers/ideas?

## RE: Questions about a finite element modeling situation ?

NRP99Yes, if I reduce my E by 84% I will get the same results in frequency. Is it correct to reduce it so much ?

## RE: Questions about a finite element modeling situation ?

## RE: Questions about a finite element modeling situation ?

However this shouldn't have any effect on mass calculation, so I don't understand why the mass is not correct: as in the corners, for the outer shell, you have twice the area, so reducing the density by 50% should give

exactlythe same figure as for the solid model (and the mid-shell model).Concerning the modulus reduction and its influence on the bending stiffness, that's less simple. The reduction of E by 50% is what one expects, at first sight, to keep the same EJ product for the whole section. However this is not entirely correct, as for the 'vertical' walls of the beam a stronger reduction of E is needed to keep the same EJ: by recalculating the whole section with 12 as the outer edge and 3 for the thickness, I get a reduction factor of E for the corners of 42%, instead of 50%.

Another factor that may affect this matter is that everything is based on the basic assumption of bending theory, that the sections remain plane after deformation: now this is likely strongly incorrect in the model with the corners having a lower E, as the 'flanges' of the section (the 'horizontal' walls) certainly deviate from that assumption (you could easily check by how much).

I'm afraid that not much more can be said or done on this subject, the solid model is the only one that may solve all the issues (but, as expected, you get a better approximation with the density and E reductions).

prex

http://www.xcalcs.com : Online engineering calculations

https://www.megamag.it : Magnetic brakes and launchers for fun rides

https://www.levitans.com : Air bearing pads

## RE: Questions about a finite element modeling situation ?

Another dimension to keep in mind before moving forward is the shaft is tapered. Any knockdown factor that may be somewhat valid for one cross section but not valid for the entire length.

Instead of modifying the corners, an

unverified suggestionis to modify the entire cross section properties (thickness, E & density) to be more like theShell_Midmodel. These values would change depending on the tapered cross section edge lengths. Perhaps you or others could comment if this approach is valid.Step 1. Adjust each shell thickness of outer-surface(OS) such that it's area is the same as the original mid-surface(MS). The thickness

_{OS}is a function of length of the tapered shaft.## CODE --> math

^{3}where the width is varying along the length of the shaft. This is done via trial-and-error/optimization. I assume a simple relationship of inverse cubic but could be wrong. A more complicated cubic or quadratic function may fit better.Step 3. Adjust the densities to match original mass.

I hope this spark some ideas.

Best regards,

Sze Kwan (Jason) Cheah