Trouble importing geometry to CFD

[Anonymous]

Hi there.

I'm importing a SolidWorks Assembly that comes from 3 parts. One of them comes from an assembly that I converted into a Parasolid and then into a part to reduce the number of parts inside it from 80 to 2. The problem is that even when I'm importing the last assembly that only have 3 parts, Autodesk CFD is generating too many parts.

The first photograph is the part that is made with 80 parts.

The seconds one is when I already converted into only two parts.

The third one is the assembly that I'm importing to Autodesk CFD

And the last one is how Autodesk CFD is generating the geometry.

Is there a way to mix or combine parts in Autodesk CFD? This because I don't want to apply the material and boundary conditions to each one.

[Jon.Wilde]

My guess is that there are a lot of small overlapping volumes and tiny surfaces that are causing an issue when you import.

How clean is the CAD model?

What is the end goal here too, how will you use CFD here?

Thanks,

Jon

[Anonymous]

Thanks for your reply.

I want to determine the loss of static pressure through a randomly stacked bulk of apples and then create an equivalent porous media to analyse the design of a forced air precooling system. With the equivalent porous media, I'm trying to reduce the CAD complexity because my computer won't run the full simulation.

The CAD model comes from an analysis of the motion of apples falling with gravity into the package. In this way I'm assuring they are randomly stacked. When I finished the simulation there were a lot of overlapping volumes, but I combined the parts to get only one solid and I assumed that the overlapping volumes would not interfere with my CFD simulation.

[Jon.Wilde]

I would guess that all the small parts are just the overlapping solids. It should not be a problem, they will all be suppressed anyway as you only need to model the one air volume 🙂

Have you tried adding a wind tunnel type air volume in CAD already? This is what you are going to need in CFD eventually I think, right? Then you can suppress the apples from the mesh anyway.

Another approach might be to subtract them from the air in Solidworks before you move into CFD, could be a little faster?

Does that help you at all?

Thanks,

Jon

[Anonymous]

I already checked the model and I found that you were guessing correctly, the model is no so clean, they are overlapping solids.

Yes, it helps me a lot. I'm going to try what you're suggesting me and then I'm going to tell you if it works. If I suppress the apples from the mesh, would not affect the static pressure analysis?

Thanks a lot, Jon!

[Amal.C]

Hi @Anonymous,

From the Output bar message, you can see that CFD has created 15 additional parts. This usually happens either when you have overlapping parts (the intersecting volumes are created by CFD) or when you have an enclosed area where CFD will fill automatically the inner volume. 

Not meshing the apples will not affect the static pressure 🙂 We usually suppress solids when we are not running heat transfer analyses to decrease the mesh count and thus avoid long run time. 

I hope this helps 🙂 

Thanks,

Amal

[Amal.C]

Hi @Anonymous,

Would you please provide an update regarding this issue? Were you finally able to import the CAD into CFD without issues?

Please let us know if you still need help! We will be glad to further assist you 🙂 

Thanks,

Amal

[Anonymous]

Hi, @Amal.C,

My apologies for not answering. I am still not capable of running the simulation, but not because of the issue that I posted here. It is because of my computer is crashing as a consequence that it does not have the minimum requirements. I am working on getting a computer that does have it, that's why I hadn't replied yet. As soon as I fix this problem and get my results, I will let you know, and I will post them here.

When I tried this simulation, first I deleted the control volume of air that I had created with SolidWorks, and I built it with Autodesk CFD. After that, I suppressed the apples and the container from the mesh as @Jon.Wilde and you had suggested me, everything was going right, but then my laptop collapsed. Right now, I am trying to clean my CAD merging the edges with the geometry tool, and I am changing my mesh from 0.3 to 0.5 with the aim of getting at least one approximation.

 What do you think about it? By the way, do you have any other idea to get the geometry that I require? This study aim is to simulate the loss of static pressure through a randomly stacked geometry of apples in a container.

Thanks again for your help, I appreciate it so much.

Best regards.

Alan Marruenda

Alan Marruenda

[Jon.Wilde]

Hi Alan,

I think at this point, as you have a model in CFD and ready to go, we might be able to help a little more.

How about saving out a support file (CFZ) and posting it here for us to run a quick test, to answer two questions:

1. How much RAM might this model need to create a mesh?
2. Is there still a geometry issue?

Thanks!

Jon

[Anonymous]

Hi @Jon.Wilde,

I attached the file CFZ. Please tell me if something is wrong or you believe that it could be done in some other way.

Thank you.

[Jon.Wilde]

I have a few ideas here 🙂

1. Model the air within CAD, so that it covers only the area you need
2. Make the inlet and outlets longer, about 5x the height of the container (should be more realistic and stable)
3. The issue is likely where you have the apples 'just' touching as CFD is going to try to mesh those small gaps, which is quite a complex process to automate. Even once meshed it will also cram in a boundary layer on both sides of the gap. It might be worth overlapping them all a little
   • A manual mesh might help work around this without you having to modify the CAD - I am testing now and I will update you a little later :)
     • (Actually it just meshed in the time it took to type this, more shortly once I have time to look at the mesh quality a little)

Thanks for sharing!

Jon

[Jon.Wilde]

Take a look at my manual mesh settings here. Note the meshing region to tighten it up a little around the apples. This sort of this should work and I think also run with 8GB of RAM (just 🙂 ).

Flow vectors here, looks OK to me!

Note that you have flow going around the box here, is that representative of what you want to test? If not, model the air in CAD.

Hope that helps!

Jon

[Anonymous]

Hi, John.

I can't open the attached file because it was created with a later version of Autodesk CFD. I am using Autodesk CFD 2017.

In this idea "The issue is likely where you have the apples 'just' touching as CFD is going to try to mesh those small gaps, which is quite a complex process to automate. Even once meshed it will also cram in a boundary layer on both sides of the gap. It might be worth overlapping them all a little" In the last sentence (in red), how can I overlap them? I think that in my CAD it would be so complicated.

Anyway, the problem with the apples (that are just touching) can be ignored by doing manual meshing, doesn't it? If it's correct, I will modify the air volume whether in my CAD or CFD to get 5x the height of the container. I am not sure if it won't affect the measure of the loss of static pressure between the inlet and outlet of the container. In my application, the air is forced to pass between the gaps in the stacked apples only. In other words, the air is not able to bypass the container (neither at the top, bottom, right or left of the container, it's completely sealed) as it looks like in the image that you attached.

Thanks a LOT for all of your ideas, simulations and the time that you have spent on this!!!

[Jon.Wilde]

No problem 🙂

I do not mean 5x the height though. Make them a little less high, so no air can escape around the edges I pointed to.

Then make them a lot longer (the length should = roughly 5x the height 🙂 ).

Does that make sense?

[Jon.Wilde · Accepted solution]

Here you go, set up and ready to go in 2017. Note again the manual mesh and the additional region.

Also added slip/symmetry to the side walls as this is not really in a tunnel, right?

This should give you pretty good results 🙂

[Anonymous]

Yes it does make sense. I'm running the simulation and it looks pretty good.

Thanks a lot!!

[Jon.Wilde]

No problem at all. Enjoy CFD and shout again should you need to 🙂

[Anonymous]

Hi again Jon,

I was working in something similar and I was wondering how did you create the control volume? Do you remember that we had this problem before?

There is a "leakage" above and below the package. I remember that you fixed that error but I didn't know how. Could you explain me?

Regards,

Alan Marruenda

[David.Short. · Accepted solution]

Hi @Anonymous,

Jon is actually on holiday at the moment so hopefully ill be able to help in the meantime (knowing Jon he'll probably reply as well anyway!!).

To avoid leakage around the package I would create the external volume in CAD rather than using the geometry tool in CFD. You can then apply a height equal to the height of the package such that flow is only directed at the package and cannot go above or below it.

Hope that helps,

David

[Anonymous]

Hi David,

Thank you for answering. That's just what I have done. I have never done it before, that's why I didn't know that it was easier to make the control volume with my CAD, in fact, is the easiest thing I have done hahahaha.

I am working with another simulation but my computer is not good enough to run it. It start to slow down even when I open the CAD in Autodesk CFD. It would be possible that you run it for me? I can send you the CFZ file ready to mesh and run. If that's possible, to see the results is going to be hard for my computer anyway isn't it?

Kind regards,

Alan Marruenda