Hey, I know a lot of you guys use Pro/E to model you chassis. Right now, I am using Insert->Advanced->Pipe. I have the chassis modeled, but whenever I try to change nodes around, tubes crash out. We were able to get around that by making redundent nodes slightly offset the core nodes and moved the crashed tubing to that node. But this is a bad way of fixing this. Also, we have tried modeling the whole chassis out of solid bar. This made the problem a bit better, but it still crashes out bar. How do other teams model their chassis in pro/e? Any tips?

After having this problem and numerous others and a three week hell we solved the problem buy buying an accademic copy of solidworks and after 5 minutes the weldment feature was our friend. It is soooooo much easyer

Model each tube and make the weldment an assembly.

This is wayyyy more efficient from a modeling standpoint because PRO\E has a hard time trying to merge the pipes at nodes.

Also you can make drawings for individual tubes and have them pre-fabricated and then just weld them in place when you are ready for them.

An efficient way to do this is to use skeleton modeling. Make a skeleton model of your nodes by using xyz points and then the lenths of the tubes can be linked to the distance between the nodes. Then if you want to move a node all the tubes that connect to the node will automatically change their lengths.

Create a file is chassis_pts.prt This is the first file to e put into the frame assembly and all the tubes are built off this. If a change is made to this file the tube files will update accordingly. This would be the first file in a chassis assembly. Then you would create the tubes in the assembly using the points in the chassis points file as references. We have not had any problems updating a chassis this way. Also be careful that any tube points that have bends do not cause any problems.

Thanks for the suggestions. Just to clarify, we did do skeleton modeling. All of the nodes were created as datum point and then the datum point were connected using the pipe feature. But you guys are saying to build the chassis as an assembly and not a single part file? Right now I did it as a part file... If I were to build it as an assembly, would I use the piping application?

You still use the piping feature in assembly mode. The assembly is composed of the first file I mentioned that defines all the points with datum points. Then the rest of the parts are each individual tube of the chassis. We create the tubes in the assembly. Instead of using the insert componenet for the assembly use the button below that to create a component in assembly from features.

You should consider using HyperMesh and OptiStruct for your chassis models. If you're running a stick model (1Ds) then it'll definitely be worth your while. Once you have the overall configuration tube configuration figured out you can easily do an optimization on your tube sizes and thicknesses to get the best efficiency out of your structure.

OptiStruct is sort of a Nastran clone with a slew of optimization sequences added. There are some differences in the codes, but it's easy to switch and OS should be more predictive for shell-meshed models. The whole HyperWorks suite is free for FSAE teams and Altair offers free training to students.

I will put in another plug for solidworks.. the 3d sketch to structural tube member feature is awesome.. I change around the frame nodes all the time and it never crashes.. plus you can do beam analysis in COSMOSworks now which are simply a breeze..

One more plug for solidworks here. So easy to do, just do a simple line drawing and then the weldment extrudes into whatever tube size you like. Once you've done it, takes very little time to reproduce another entire chassis and as said very simple to modify.

has anyone else had problems with roll hoops in the CosmosWorks2007 Beam Analysis? According to the help menu and my experience, it can only analyze straight beams.
Unless i'm missing something, this package isn't as useful as i was hoping it would be.

I tried to do our chassis for a while in COSMOS and it would give me error after error. So we went back to our tedious ALGOR model instead. It would have been awesome not to have to manually enter every point in the chassis like in ALGOR, but I would get a multitude of errors.

quote:

Originally posted by Anday:
has anyone else had problems with roll hoops in the CosmosWorks2007 Beam Analysis? According to the help menu and my experience, it can only analyze straight beams.
Unless i'm missing something, this package isn't as useful as i was hoping it would be.

Yep, we had to convert our roll hoops to triangles to get it to work.

From my expirences it only does straight beam.. failes to snalyze anything I've tried that has a curve.

I've gotten Pro-E to work. I started with a wire model of our frame (using curves in "Standard") then turning that into beams using Pro Mechanica's simulation feature. You'll need to create saved beam sections for this to work (I used saved sections from our CAD library) but its pretty straightforward once you figure it out.

I did have to go back once the frame design was settled to make a rendering using solid pipes and that was a bit tedious, but that's how I got a model to use for placing components (ie I just used 1" thick pipes for everything so we can see fitments and such)

I'm trying to figure this out right now. I made a part file with datum points and brought that into an assembly file. Then I click 'Create component in Assembly' - 'Insert' - 'Advanced' and the pipe feature is grayed out. If I don't click on the 'Create component in assembly' and just go to 'Insert' - 'Advanced'-'Pipe...' it works but only shows a trajectory.

How do I get it to show the pipe? How do I make it a square tube if I want to? Or when I make the pipes in the part file with the datum points is there a reasonably easy way to blend or "fishmouth" the tubes in there?

I have a feeling our team is going to pick up a copy of solidworks

Thanks

Does anybody know if somewhere on the web is there any guide or tutorial on modelling Chassis components like this with pro-e?

We figured it out. I'm not in the lab right now but this should be very close to the actual steps...

When you already have your motion skeleton modeled, bring it into an assembly and...

-Create component in assembly
-Either create features or no features (whichever one doesn't have a line to type in or a drop down menu)
-Insert
-Sweep
-Thin protrusion
-Sketch geometry (haven't figure out select geometry in an assembly yet, only for a .prt)
-select the line you want to create a tube around
-create datum
-through
-i think now you just middle click 2 or 3 times and then it goes into a sketcher view
-create your OD dimensions hit the check button(1" circle for example)
-then I think you have to tell it the wall thickness but make sure the arrow on the circle you just created is pointing toward the center of the circle before you enter the wall thickness. Otherwise it will make a 1.095" OD tube for example.

I think thats it but I'm not positive. If you still have problems pm me and I'll get back to you when I'm in the lab.