×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Are you an
Engineering professional?
Join Eng-Tips Forums!
• Talk With Other Members
• Be Notified Of Responses
• Keyword Search
Favorite Forums
• Automated Signatures
• Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

#### Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

# 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.

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

1) why do you Have to use the external surface for some shells ? You Can always measure to the OML, then calc where the mid-surface is; and these are flat shells (ie 4 points per surface)

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)

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

(OP)
1) Because of the design of the part I had to use exterior surface on those beams to generate the shell elements, it was easier for me to construct the model because you have other beams and plates intersecting with this one. I don t really understand what OML means?

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 ?

1) OML = outer mould line (the outer face) I think you're using the external face of the part for your model because it's easier for you. It doesn't look to be a lot of work to extract the midplane. This will affect the weight of the model, if that's important to you.

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.

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

(OP)
1) Yes, the shell elements are constructed at the outer surface of the beam. It would be easy to construct the mid-surface but it would take very long because there are a lot of things (connection with other beams, plates, etc.) to be modified/resolved, and I don't have the time because the project is ending soon

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 ?

Hi Ionut,

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 rb1957 where 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 ?

1) the project ends when the work's done !

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 !

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

Ionut Cosmin

1)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 ?

Assuming your beams effectively react as 'beams' (normal stress + bending stress), then you need to divide by 2, in the corners, not only the density, but also the elastic modulus of the material. Otherwise, using 12 as the side and 3 as the thickness, you would get an increase of 33% in axial stiffness and of nearly 50% in bending stiffness.
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

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

(OP)
Jason

I 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.

rb1957

1) 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

NRP99

Unfortunately 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.

prex

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

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

sorry, I thought the overlap was on the face of the elements, not in the thickness.

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)

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

(OP)
rb1957

Yes 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 ?

prex

#### Quote (prex)

Assuming your beams effectively react as 'beams' (normal stress + bending stress), then you need to divide by 2, in the corners, not only the density, but also the elastic modulus of the material.

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 ?

(OP)
Okay guys I have run some simulations on a single beam modeled with solid elements, shell elements on outer layer and shell elements on mid-plane. The models can be seen here. The beams are blocked in translation at one end and a mass (CONM2 property) was tied using RBE2 at the other end.

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 Cosmin

At 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 ?

(OP)
NRP99

Yes, 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 ?

I guess so. Solid model will reflect your actual condition. All other models will be approximate than solid one(even solid also approximation to real but comparatively close to real than other approaches).

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

Sorry Ionut, I am not sure to understand how the shell offset feature really works.
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 exactly the 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

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

Ionut,

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 suggestion is to modify the entire cross section properties (thickness, E & density) to be more like the Shell_Mid model. 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 thicknessOS is a function of length of the tapered shaft.

#### CODE --> math

widthMS*thicknessMS = widthOS*thicknessOS
widthOS = widthMS+thicknessMS
thicknessOS = widthMS*thicknessMS/(widthMS+thicknessMS) 
Step 2. Determine the modulus of elasticity scale factor for the cross section that is proportional to inverse of width3 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

#### Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

#### Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Close Box

# Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

• Talk To Other Members
• Notification Of Responses To Questions
• Favorite Forums One Click Access
• Keyword Search Of All Posts, And More...

Register now while it's still free!