Autodesk Inventor Chassis model

[PeteG]

Has anyone got any tips on modelling a space frame chassis in inventor? we've just spent all afternoon trying it and its all over the place. We're thinking weldments or 3d sketches might help? any help would be great

pete

[PeteG]

Has anyone got any tips on modelling a space frame chassis in inventor? we've just spent all afternoon trying it and its all over the place. We're thinking weldments or 3d sketches might help? any help would be great

pete

[Denny Trimble]

We use SolidWorks, so I don't know if Inventor can't do any of these steps, but here's the general process:

1) 3D sketch of nodes connected by lines (wireframe)
2) Create a tube profile sketch at the midpoint of each line and extrude to the nodes
3) If you really want to be fancy, revolve a sphere at each node to fill in the gaps.

The benefit of starting with a wireframe model is that you can export it to ANSYS or Algor to do beam-element FEA, which is very computationally efficient.

[rjwoods77]

Adding to what denny said. I use solidworks as well. Not to say that inventor is bad but I made the switch and glad I did.
I setup an entire wire frame to start with. The best way to do a wireframe is to set up planes all over the place and then use 2d and 3d sketchs that constrain against those planes. The nice thing about this is that when you want to modify the wireframe to all you have to do is change the defenition of the planes(offset from origin planes). This works great because when you want to tweak stuff all you have to do is change one plane and it will update any number of connected wireframe lines. Definitely the way to go. I made a fully adaptive frame in solidworks. I finally got it to work correctly too.

Once the wireframe is set then all I do is place a plane "normal to the curve". I draw the profile of the tube circles and sweep it on the wireframe line. So it goes (plane,sketch,sweep). Denny suggests doing it to the midpoint of each line but I dont know how he is doing it. Different version maybe. I always start at one end of the line/curve. I also have alot of bent tubing in my frame so finding the midpoint of a sketch line isnt always an option.

If you really want to get fancy with tube notching then what i have done in the past is to use the tube profiles of intersecting tubes as the profile to extrude cut a notch in the corresponding tubing. The profiles of the intersecting tubes can be used to notch the tubing out. But this isnt really a good idea.

It will make your computer crunch alot more which drives me nuts when i am trying to get stuff done. Also I have found if you dont notch and dont put a weld in the assembly that the weight of that frame without any of the notches ends up close to the notched and welded frame. So I just use that assumption and save my computer the heartburn. Up to you though.

The latest version of solidworks(2005) is sick. It has some features that make spaceframe development a dream. Now that version blows inventor out of the water. Early versions are closer in comparison.

[Denny Trimble]

Right, I forgot you can't select midpoints in 3D sketches. Here's a tip though: CTRL select an endpoint and a line, then create a sketch. It will automatically create a plane on the endpoint normal to the line, which is what you want, and create a sketch on that plane. Makes things go a little faster.

[Lyn Labahn UW-Madison]

Solidworks 2004-2005 has a weldments feature that allows you to do a 3d sketch, and then select the line and apply a tubing size to it. It will even do pretty end copes against other weldments! The only down side is that you have to create your own profiles, but that shouldn't take more than 15 minutes and it only has to be done once! To switch a tube size or thickness, you only need to edit the feature. It cannot do bent tubes, such as rollhoops however. I hope that in future versions you can,

[rjwoods77]

Hey Denny,
I keep running into this problem with 3D sketches. The colors show everything contrained. Nothing will move but in the feature tree it shows that the 3d sketch is underdefined. Its always on 3D sketches. Nothing ever moves so it is alright but it just makes me insecure about my sexuality. (Big joke around our team. Something isnt right=insecure sexuality)

[Denny Trimble]

http://students.washington.edu/dennyt/fsae/3dsketch.jpg

2004-2005 Student Edition, fully constains just fine for me. Yup, you're gay.

[rjwoods77]

Yeah I know. Just been trying to figure out how to tell my family. hahahhahahahahaa. Yeah, I know how the feature tree is suppose to look but all the lines are black and nothing can move. I've been meaning to by that version of student software. Powerfull stuff with the extra cosmos programs.

[fsae racer]

Hey Pete, I struggled with your exact task for a solid 12 hours straight one day. I was trying all kinds fo crayz shit like making each tube an individual .ipt. The next day it just dawned on me. I made all the box tubes in the suspension, then I just started making 3d sketches like you mentioned. One of the key things to remember is to include user defined work points. That will allow you to define new 2d sketches with a line and the point. draw your cross sections on that new sketch, finish the sketch, and profile the 3d sketch. One thing to watch our for though, always profile immediately after creating your cross section because if you attempt to make a new 3d sketch that crosses over the one you just made, the profile path will continue on the new 3d sketch. If your confused, lemme know and ill see what i can come up with. Last years' team captain took like 6 months to do the whole frame bc he didnt do it this way. I did the whole frame with all the suspension point, shock mounts, bellcrank axes, and control arm pick-ups in 2 nights with the method i described above. good luck, nick.

[Frank]

wait until you try basic surface modeling

or variables "linking" to inventor to drive designs

comparing inventor to solid works / solid edge

is like comparing duplo to lego

its retarded software for autocad gumbies needing 3d trainer wheels

i really hope an "inventor" vendor reads this

it is really heavy on system resources too (ive heard this is fault of the modelling kernal itself, but i dont understand that at all)

i watched in horror as a so-called "professional v888 touring car team" fumbled with this rotten package

[David H.]

Hey guys, just wondering if one of you could send me your Solid Works frame file. I'm really interested in how you go about doing this in SW and also the technical basis of an FSAE frame. And no im not going to steal your work and claim it as mine =P I'm just trying to get a start on this project w/ my very limited knowledge.

[Rob Davies]

I too am having pissy fits at Solidworks as it seems so darn hard to make a simple chassis.

I generally have about 100 planes in just the rear chassis

Whenever I make a wire-frame that has wires coming in from different planes then Solidworks complains at me....

And then when suspension changes their pick up point it takes me a good day to change the model..

Anyone with some SolidWorks tips will be very appreciated.

Thanks, Rob

[Mike T.]

I find it easiest to extrude the tubing profiles in both directions from a point somewhere close to the midpoint of a 3dsketch line using the 'up to next' end condition. This basically simulates a notch, and the tubes fit perfectly together without overlapping. Doing it this way also makes you think about the order in which you'll actually place the tubes when manufacturing, which is a good thing. It also allows you to get accurate mass properties. I've put together a simple model in Solidworks 2004 to illustrate this, just follow the link:

http://students.washington.edu/trumbore/TubeframeExample.SLDPRT

If you set it to wireframe view with hidden lines, you can see that the tubes fit perfectly up to one another without overlapping.

The solidworks help files can be quite helpful as well when it comes to figuring out what you can do with features and end conditions and such.

I've messed around some with the new weldment features in 2004, and haven't found them to be of any help since it's a bit tough to simulate many tubes fitting together, which we often have on our tubeframes.

Hope this helps out,

Mike T.

[Rob Davies]

Cheers Mike Great Help

Thanks, Rob

[Courtney Waters]

Like Mike said, extruding from the middle of a line works well. Simply create a plane normal to the curve (line) at one endpoint, then offset a new plane X amount to get near the middle of the line. Make your tube profile on that plane and extrude to body in both directions (or whatever extrusion option you prefer). This doesn't work for swept features though (which sucks when you want to do a bent tube). Maybe that's been addressed in the lastest version, I don't know. Getting SW to let me make drawings of the tubes with dimensions of the relative angles of the notches has been a PITA though.

On the Inventor vs. SW comments, I don't see why it would be considered "3d training wheels" for autocad users, at least not any more than SW. Functionally it is nearly idendical to SW. It's not like you are using a command line to input commands (though that is an option). Inventor uses all the same concepts as SW (planes, sketches, various extruded features, parts, assemblies, blah blah). I haven't used Inventor on a regular basis for the last year or so since I left school and we use SW at work, but I found Inventor to be more user-friendly than SW in a number of respects. Yes, SW has some superior features, but for all it's "glory" SW is far from perfect and I find myself calling it SolidQuirks as often as not.

[Cement Legs]

<BLOCKQUOTE class="ip-ubbcode-quote"><font size="-1">quote:</font><HR>Originally posted by Denny Trimble:

The benefit of starting with a wireframe model is that you can export it to ANSYS or Algor to do beam-element FEA, which is very computationally efficient. <HR></BLOCKQUOTE>

Ahhhhh... we have had a heck of a time trying to get an accurate FEA done on a frame designed in Unigraphics (absolutely love it). When I set the frame up as solid members I can get an FEA (with unigraphics) completed but when I build the frame with hollow tubing I get all kinds of Boolean operation errors, probably from infinitely small gaps or "0" thickness measurements after subtracting solids. Anyway, I gave the model file to a friend who does a lot of FEA and he tried it on Algor but again it would run for about 8 hrs then crap out. I was not aware that you could set it up with wire frame and assign it "beam element preperties". Could you explain this a little further so I have my ducks in a row when I go back to this guy and ask for more of his time. http://fsae.com/groupee_common/emoticons/icon_smile.gif

PS if you guys are having trouble with solidworks and have access to Unigraphics give it a try. The learning curve is a little steep, my first frame took me about 2 weeks to create after the design was done, I've got it down to less than 30 min now if I know all of the points.

[rjwoods77]

I dont understand why you would offset a plane to the middle of a line segment to extrude the tube. Wether you draw a line segment to sweep with a 2D or a 3D, it would be easier to put a plane tangent to the curve which places the plane at the end of the segment. Less steps involved. It also places the tube cutting profile right at the node. Mike T. is right also. You may curse the program for this and that but it is your lack of understanding that is the problem. Trust me. Took me about 2 months to get it all sorted out. Now it is smooth as silk. Almost.

[Rob Davies]

Courtney,
Did u find a way to make SolidWorks produce a drawing of an individual tube as I was trying that the other day.

Rob

[Denny Trimble]

<BLOCKQUOTE class="ip-ubbcode-quote"><font size="-1">quote:</font><HR>Originally posted by Cement Legs:
I was not aware that you could set it up with wire frame and assign it "beam element preperties". Could you explain this a little further so I have my ducks in a row when I go back to this guy and ask for more of his time. http://fsae.com/groupee_common/emoticons/icon_smile.gif
<HR></BLOCKQUOTE>

Beam element FEA is really simple. You export a 3D wireframe model (IGES works, with the right options turned on). Then you set up layers (depends on the FEA software) for different tube sections, i.e. 1" x .095 wall round tube. Then apply the tube properties to the appropriate lines, and you've got an FEA model. Look into the help or tutorial for your specific FEA package.

On the modeling front, make sure that all your line segments end at tubing nodes. One pitfall is a long tube with a node in the middle, where other tubes connect to it. Most FEA packages won't connect the other tubes to the long one unless the long line is split into two shorter ones, ending at the node.

Play your results back in "Animate" mode, and look out for that.

[Allen]

<BLOCKQUOTE class="ip-ubbcode-quote"><font size="-1">quote:</font><HR>Originally posted by Denny Trimble:

Beam element FEA is really simple. You export a 3D wireframe model (IGES works, with the right options turned on). Then you set up layers (depends on the FEA software) for different tube sections, i.e. 1" x .095 wall round tube. Then apply the tube properties to the appropriate lines, and you've got an FEA model. Look into the help or tutorial for your specific FEA package.

<HR></BLOCKQUOTE>

Hey Denny, I am using ALGOR, modelling in SolidWorks, and was wondering do you import the IGES wireframe into Superdraw 3 or straight into FEMPRO? I have this feeling that the ALGOR we have might be a crap version since I can't open IGES files in FEMPRO even though the tutorials say otherwise.

[Denny Trimble]

Oh yeah, you have to open up Superdraw, "import cad wireframe", then "export to FEMPRO". That works with the version they gave us last year.

Other funny business:
-Loads and restraints don't reappear if you save, close, and open.
-Saving before running sometimes causes crashes, so I usually import the wireframe, add tube properties, save and exit, then open it back up, add BC's, and run it, get all the info I need, then save and move on to the next iteration.
-Try rearranging the toolbars so they take up less space. They're possessed!

Hope this helps,
-Denny

[Lash]

Has anyone successfully done FEA in COSMOS WORKS ? This isn't the COSMOS that comes with solid works it is the full version FEA package you buy as a set. Let was suscessful in performing FEA.

Trevor

[Allen]

Denny,

Do you import the wireframe and export right away? Or do you add the tube properties in Superdraw? I get major geometrical problems when I export an IGES directly into FEMPRO. By the way, how do you add tube properties, or can you reference me to a place where I can get this information?

As for the possessed toolbars, it helps making the icons as small as possible... but they're still crazy.

[Denny Trimble]

Allen,
I went straight from Superdraw to FEMPRO after importing the IGES file. I didn't have any IGES problems, but I don't know if you started with a SolidWorks model like I did. Most CAD packages have IGES export options, try playing with those.

For assigning tube properties, here's how you do it:
1) Get your wireframe into FEMPRO (see post above)
2) Select Element Type - Beam (right-click)
3) Select various tubes, right-click -&gt; modify attributes, assign to layers (so you have layers to assign properties to in the next step)
4) Right-Click on Element Definition to get to the dialog box. Click a layer, hit the "cross section libraries" button, select "pipe" or "hollow rectangular", specify OD and ID, and off you go.

Have fun.

P.S. I just got a "cannot read memory" error when canceling out of one of those dialog boxes... quality software http://fsae.com/groupee_common/emoticons/icon_rolleyes.gif

[Allen]

Hey Denny,
I was trying it out, but I kept getting problems. I am using SolidWorks. You can go here to check out the steps I made:

http://www.xanga.com/home.aspx?user=zzyx7

ah... gotta love free webspace http://fsae.com/groupee_common/emoticons/icon_wink.gif.

Anyways, when I first imported, the wireframe was waaaay zoomed out. I zoomed in and got the mess of lines in the 3rd pic. I don't know if it's my IGES settings or what, but I tried to clean things up in the 4th pic.

Then I set up all those lines into 3 layers, and set the round pipe OD and ID for them all. I ran the analysis and ended up with 'model contains errors due to geometry problems' message about 2 secs into the run.

I tried to have fun with it, but ended up with a headache... can you help me out?

[Denny Trimble]

Allen,
I can't see the images, it appears they're linking to your C drive, not on public webspace.

I forgot to mention that ALGOR doesn't like lines that aren't straight http://fsae.com/groupee_common/emoticons/icon_smile.gif You can either turn your tubing bends into straight line segments, or use the "divide" command in superdraw to do so. We've had more luck doing it ourselves, as the divide command doesn't work perfectly.

A case of beer should help with the headache...

[jdstuff]

Hello Allen,
Denny is right about ALGOR throwing a fit about arcs and circles. Breaking them up is the best way to go. Also, as much as I hate to say it, we usually get the best results by just drawing our chassis from scratch in Superdraw. We pick off the nodal co-ordinates in Solid Edge (which we use to model the chassis in the first place) and make a spread sheet, then reconstruct it in Superdraw. This may take a little longer up front, but once you build the first model done it isn't too bad. And I've found that I actually spend LESS time overall than trying to import/export IGES files, and dealing with all the little quirks. We usually get 2 people working in tandem (one skilled with Solid Edge and one with ALGOR), which makes iterations go quite a bit quicker.

And Denny....
A case of beer will definately do the trick, but we've also found that a 4' section of 4130 .065" (dubbed the beater-stick) that we stole from Baja works in most situations. It is especially effective in breaking old flourecent lightbulbs and large glass jars. http://fsae.com/groupee_common/emoticons/icon_wink.gif

[alfordda]

Jason-

How are you drawing the frame in SE? We have been using the curve by table command to create the wireframe, and then extruding the tubes along those lines.

[Allen]

Ahh, turkey is good...Hope you all had a good Thanksgiving break http://fsae.com/groupee_common/emoticons/icon_smile.gif

Denny, sorry for the image problems... try this:
http://pg.photos.yahoo.com/ph/zzyx7/my_photos
The pics should be under the "FSAE" album.

Jason, I drew the frame in Superdraw the way you described, but I still get geometry errors. I made a simple box with 1x.035 steel tubing. It's at the same link above but under the "ALGOR box" album. This box has the same problems. I thought the box would error free since there's less geometry, but I get the same error. Do you guys have to mesh anything?

Thanks,
Allen

[Denny Trimble]

Allen,
Uncheck the "IGES solid/surface entities" box in the IGES output options. You only want to send Algor your wireframe (centerline) geometry, not the entire tube surfaces.

Actually, that should give you the same result as drawing it up in superdraw, and if you're still having problems, I don't know what the deal is.

Feel free to email me your sample files if you like, dennyt at u.washington.edu.