Hi there, We think of buying Icem with the direct Catia interface, to avoid these timeconsuming geometrycleanups. Does anybody have experience with this interface and can tell me about it (how and if it really works...)? Would be great, thanx in advance

Dirk

Dirk,

Yes it does work and we have lot of users in the UK who are happy with it. There is a stand alone reader and a fully embedded CATIA interface. Contact your local ICEM office for more info.

Caroline

I have not used the interface to CATIA, only to UG, but I assume they are similar. It works very well , but a problem is the tolerance in the CAD-tools. Generally the tolerance used for CAD is much larger than required for CFD. For example when trying create a mesh with resolved boundary layers in ICEM the tolerance between surfaces were at least one order greater than the cell size at the wall. So there might still be a need for geometry cleanup, or even remaking the model, in order to get good geometry with small enough tolerances. The geometry tools in ICEM can do this, but they are slow to use and it is very tedious. Besides, you get a lot of small surfaces filling in the gaps, instead of extending the surfaces already there. Very annoying. So don't expect to much from the interfaces.

But good luck.

Martin

Martin,

We have never had a UK user who has had this problem perhaps you should look at your tri-tolerance, it should be 0.001 or 0.0001.

If you still have problems contact your local ICEM office as you should not have to use CAD repair at all.

Caroline

I think that the problem Martin refers to is before you create your tetin file (your surface triangulation). I have seen the same problem often myself - when you extract your UG surfaces in the direct interface they "fall apart", even though they look perfect inside UG (the surface intersection might even be the result of a "sweep" operation in UG, and thus should be perfect) - the surface description inside UG is simply not good enough to serve as a basis for meshing resolved boundary layers in ICEM - when you get it into ICEM you get an edge and two surfaces which do not match perfectly. Decreasing the tolerances inside UG helps somewhat, but it is still a very tedious work.

We have started going the extra way over STL to solve this problem with the direct CAD interface to UG.

Even if I change the tolerance on the CAD-geometry I import I cannot recreate any smaller tolerance that was not there when the surfaces were made. This is not a problem with ICEM itself it is just an issue that arises when using surfaces primarily intended for other purposes than CFD-simulations. CAD surfaces generally have much greater tolerance than the cell sizes sometimes needed. The point I wanted to make is that one should expect some work on the geometry before being able to use it for meshing, especially if you want to resolve the boundary layer (small cells close to the walls). When I used the boundary layer equations and placed the first node at about y+=30 I did not have any problems as the cells then became larger than the tolerance.

Martin

Was Jonas said above was my point exactly. In fact he wrote his message while I was writing my post so I kind of say the same thing as he is.

Martin

Hy, I think I do not understand your problem really. You have problems with the tolerance of the cad-system ? That's usually something of 1/1000 mm and that that is not fine enough for you ? Don't you have the normal and various material-roughness with this numbers which are not at all reprensented in the cfd-model ?

John

For a typical application, let's say in the low pressure turbine of a jet engine the exit temperature is about 800K which gives a viscosity of 80e-6 m2/s circa for air.

If you want to resolve the boundary layer you want your first node to be placed at y+=1 and since

y=(y+*nu)/u*

you quickly realise that the friction velocity must be around 80m/s for y to be in the order of 1/1000mm. And that is not always the case. So, no sometimes the CAD tolerances are not enough. Besides, the standard tolerance in most CAD-system is one order or so greater than the 1/1000mm. It may be possible to set it lower but when a CAD part is made that is rarely the case. Draftsmen and designers often do not think of CFD simulation geometry requirements when they model a part.

Martin

That brings up another question. What tolerance do you have when producing the real geometry. It seems possible that you like to perform your simulation on a geometry which slightly differs from the product

That is not really the issue here, the issue is that in order to create resolved boundary-layers in a corner you need to have two surfaces and a corner-edge which all match perfectly (to a tolerance smaller than your smallest grid-spacing), otherwise you end up with lots of technical problems when projecting your grid onto the CAD surfaces/edges. If the CAD surfaces agree perferctly with the final product is another question which I'm less worried about - a small error here is usally no problem.

My experience with the direct interface in UG though is that when you "extract surfaces" into icem you can easily get gaps of up to 1 mm between your previously perfect surfaces - a couple of orders of magnitude greater than the smallest grid spacing needed to get y+ around 1.

1) My experience is that the interface works well. 2) But there is another point to mention. Wether you have a direct interface or not. In any case you have to clean up your CAD data. When you have a direct interface you have to do this work in your CAD system. If you do not have the interface you have to clean up the data with a cleaning up tool which should not be ICEM because there a better tools for this task. 3) I have both possibilities. My experience is the following. The clean up in the CAD system takes much longer compared to using a tool like ANSA (refer to http://www.beta-cae.gr/ or http://www.lasso.de/de/swansa.html in Germany). 4) The process with ANSA would be: a) export your CAD data into IGES or VDA format b) import these data into ANSA c) clean up your CAD data d) create an appropriate triangular surface mesh e) create your volume mesh directly within ANSA (tet with prism layers) or f) export the triangular mesh in NASTRAN format g) import the mesh into ICEM 5) This is our day to day process and it works very well. Also the tolerances ar no problem because we normally work with a turbulence model connected with a wall function. 6) When it comes to license the direct interface or ANSA you have to mention that the CATIA interface costs about 2500$ and ANSA about 10000$ per year (But ANSA is much more than an interface). But for exact prices you should contact ICEM and ANSA.

1 mm is really a big thing and a big problem also. Although I normally work with wall functions our normal height of the cells connected to the wall is between 0.5 mm and 2 mm. So a 1 mm gap would also be a problem.

1/1000 mm ? 2d/3d ? How much cells ? What's your s/l ? Sorry, such numbers (1/1000mm...) are completly unknown in my job...

If I understand correctly, you are sugesting a path of CAD->IGES->ANSA->surface mesh->ICEM CFD. Since ICEM CFD has a direct reader for CATIA model files, you can go directly from CAD to ICEM CFD, skipping the pitfalls associated with IGES and the required clean-up after the fact. For most models, clean-up is not required, and ICEM CFD does not require that you have a surface mesh in order to generate a volume mesh.

The issue of very tight tolerances for N-S meshes is a separate issue, which I will address in a separate thread.

The issue of CAD tolerances being too large for N-S meshes is a familiar one. Most ICEM CFD users creating N-S meshes with very tight near-wall spacing are using ICEM CFD Hexa. ICEM CFD Hexa has a meshing parameter called 'projection limit' intended to allow near-wall spacing which is smaller than the imperfections in the CAD model. Explaining how this works takes a bit of hand waving, but the bottom line is that the geometry is resolved within the tolerances of the CAD model, while allowing near-wall spacing significantly tighter than those tolerances. If you have questions, please feel free to contact support@icemcfd.com.

1) Yes, you are right if you understood that I recommend the indirect process via Iges and a surface mesh. 2) My point is, that it takes to long to perform the clean up work within the CAD system. 3) With clean up I do not mean filling holes or gaps. That of course is a thing which you would avoid when using a direct interface between CATIA and ICEM. 4) My clean up means the work to be done to lets say extract the inner surface of an air duct from the original CAD model. Additionally simplifications of the geometry are neccessary quite often if you want to get rid of details which would make it very hard to generate a high quality grid in ICEM Hexa or a mesh with prism layers. 5) I see that this way of working on CAD data seems a bit strange to someone who is interested in accurate CFD results. But in the automotive industry accurate results are often not needed.

Thanks for the reply. It helps to know you are working with automotive examples and that we are talking about geometry simplification, not repair. I still don't understand your desire to go through IGES. True CAD integration provides an opportunity to do de-featuring at the CAD model, where it's easy to suppress fillets and holes, for example. It's true that most automotive engineers don't have the CAD expertise or access to the parametric models in order to accomplish these tasks at the CAD level. Regardless, I would still find it preferable to export good quality surfaces, rather than go through IGES.

You may not be aware of some of the newer simplification tools in ICEM CFD. Repair and simplification of CAD and STL geometry (or other triangulated representations like VRML) has been a focus of development over the past two years. For example, ICEM CFD has a convex hull or 'shrink wrap' feature which can be used for developing simplified geometry representations.

Finally, ICEM CFD's Tetra and Hexa meshing modules are both patch independant, meaning the mesh structure is completely independant of the underlying surface topology. Put another way, there is no need to resolve every edge of every surface of your CAD model. You can selectively capture or walk over details in your surface model.

This was one of those magical little tricks that I didn't know about... I have experimented a bit with this 'projection limit' setting (available in HEXA/Meshing/Mesh/Meshing options) and it does indeed seem to help a lot - If I set the limit to 0.1mm and turn down the tolerances inside UG as much as possible things work perfectly. With this setting I was able to mesh a for us typical geometry with the first node well below y+=1 (normal distance 0.01mm). With projection limit set to 0 this has been completely impossible. THANKS for this tip - no more STL detours for me!

I have one minor complaint left with the direct interface to UG though - when you do "extract surfaces" your volumes inside UG are destroyed and you have to be carefull so that you don't save your UG part after you have done this - a bit inconvenient.

I posted a reply in the thread below, but I'll post here to be sure you're notified as well. I think the answer you're looking for is the 'projection limit' meshing option in Hexa. Set the projection limit to a value somewhat higher than the tolerance-based imperfections in your CAD model and you will be able to get good quality mesh even with very tight near-wall spacing. It sounds like Jonas had some success with this.