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Sun Jan 25, 2009 8:14 pm Post subject:
Designing a chassis, but forsee problems-how to unroll tube? |
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Hey Steve,
I've been following the La Bala builds for a while now, with some amount of jealousy  I've been kind of stalled on my own project for a while and your story is always a source of inspiration - thank you.
I've finally got the chassis looking how I want it to, and its pending an FEA shortly. I'm seeing problems building it though, how to make the angled cuts that angle in 2 dimensions (like a compound angle, I don't know how else to describe it..) Then I remembered your trick, with making paper templates that show exactly how the ends need cut (genius!)... So, my chassis is drawn in SW, but how do I convert a square tube (done as a weldment) into sheet metal?
I was reading about it here http://www.grabercars.com/phpbb2/viewtopic.php?t=1615&start=20
I appreciate any help you or others can give, thanks!!
jesse
....as soon as i figure out how to post a pic, i'll put one up =) |
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| Posted:
Mon Jan 26, 2009 9:48 am Post subject:
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Can't see the image as it is asking me to create an account. Too many of those already!
My trick is to draw a line on one of the flat surfaces of the tube. Then convert to sheet metal and rip the tube along the line that has been drawn. Finally I unfold the tube using the flatten sheet metal command. This only works for square or rectangular tube, not round tube. For round tubes I use a program called winmiter.exe (you can search google for the free download).
Hope that helps!
Steve
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Mon Jan 26, 2009 10:04 am Post subject:
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Haha, I don't blame you.. seems like there is an infinite # of forums out there..
That sounds like a winner to me, thank you for sharing! I'll give it a shot later tonight.
I'll put a pic up on photobucket or something and add that later too. Was trying to get a kind of virtual walkaround outputted from SW in mpeg or avi to put on youtube as well.
Next will be the FEA, I'm just learning Cosmoworks now, kind of sitting in on a class at my local university. So far I can't even get it to mesh, every tube fails  Need to try it with a beam mesh next, hopefully in tonight's class.
jesse |
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| Posted:
Tue Jan 27, 2009 10:13 am Post subject:
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Okay, was able to unfold a sample tube using a SW standard cross section, no problem... but I'm having a hard time getting my tube with my cross section to convert to sheet metal. It seems like it doesn't like my wall thickness maybe (0.06")? Or maybe the way I did the corners (used a simple formula from Machinery's Handbook or something similar..)?
I'll play with it more tonight, but I'm thinking its something to do with the bend radius that the sheet metal wants to follow versus the inner and outer bend radii that I specified for my cross section. Using the formula for the difference in bend radius, (i think it was just 3 x wall thickness), you obviously get a thicker spot at each 90* bend... which may not translate well to sheet metal of a set thickness. I'll try it again and just use the wall thickness as the radii difference.
I was also thinking, for your round tubes, could you just make a cross section that was essentially round, but had tiny flats (4), 90* apart? Then rip along a flat and do as you said.. maybe |
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| Posted:
Tue Jan 27, 2009 10:27 am Post subject:
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| sbcrx007 wrote: | Okay, was able to unfold a sample tube using a SW standard cross section, no problem... but I'm having a hard time getting my tube with my cross section to convert to sheet metal. It seems like it doesn't like my wall thickness maybe (0.06")? Or maybe the way I did the corners (used a simple formula from Machinery's Handbook or something similar..)?
I'll play with it more tonight, but I'm thinking its something to do with the bend radius that the sheet metal wants to follow versus the inner and outer bend radii that I specified for my cross section. Using the formula for the difference in bend radius, (i think it was just 3 x wall thickness), you obviously get a thicker spot at each 90* bend... which may not translate well to sheet metal of a set thickness. I'll try it again and just use the wall thickness as the radii difference.
I was also thinking, for your round tubes, could you just make a cross section that was essentially round, but had tiny flats (4), 90* apart? Then rip along a flat and do as you said.. maybe |
I will take a look at my sheet metal unfold settings tonite and let you know. I did have to experiment with the bend radii to get it to unfold properly for my .065 wall tube. Also, I tried for days to unfold a round tube exactly as you have suggested, but it never ever worked and I gave up. If you can figure that out I would really appreciate it!
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| Posted:
Tue Jan 27, 2009 11:24 am Post subject:
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Thanks, much appreciated!
I'll take another look at the round tubing.. Best thing might be to try and build such a tube out of sheet metal first, then try going backwards, just to see the process.. I haven't had much experience with the sheet metal features yet, but if I find anything out, I'll certainly pass it along! |
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| Posted:
Tue Jan 27, 2009 5:31 pm Post subject:
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First I create a 2d sketch on a plane using one flat side of the tube.
I use center snap from side to side so that the line I draw is parallel to the tube. I don't think you want to be ripping at an angle, but I could be wrong.
I exit the 2d sketch and in the toolbar select the 'Rip' tool. The rip parameter is the line just drawn and nothing else. I leave the default gap. Then OK. That should split your tube.
The next command is sheet metal 'Bends'. The parameters are a radius of 1/8" and Bend Deduction of 0". Then OK. The trick is to select one outer face next to your rip enter your radius and then OK.
It will create Sheet-Metal, Flatten-Bends, Process-Bends and also Flat Pattern (suppressed). I found that the easy thing to do is to unsupress flat-pattern. Magically your tube will flatten itself in the part file. But you don't have to unsuppress the flat-pattern.
Now you can start a new Drawing Sheet from this part. When you insert the part into the sheet, your choices are top,side, isometric, etc. But now you also have a choice to insert the flat pattern. Insert it onto the drawing sheet at 1:1 scale.
Done.
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| Posted:
Tue Jan 27, 2009 8:13 pm Post subject:
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That worked PERFECT! Thank you! I think all I was doing different was selecting an inside face, and I left the radius and bend deduction as default...
 Thanks! |
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| Posted:
Tue Jan 27, 2009 8:50 pm Post subject:
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If you already have your round tube joint angles figured out for the winmiter program you mentioned, maybe this would help:
Start a sketch and draw an arc that goes just short of 360 deg, with a diameter of the ID of your tubing
Insert a reference plane that is parallel to the original, at a distance of the longest length of the tube you are modeling, and enter a sketch
Highlight your 1st sketch and convert entities, exit sketch
Move to the sheet metal tab and select lofted bend, select your first and second sketches, specify thickness as your wall thickness, click ok
Now you have an unfoldable cylinder that is slit.
While folded, use extrude cut in the features tab to shave off the material that you need removed - might require a few creative reference planes and some construction only sketches to get your extrude cut direction.
Seems to work just fine, albeit a bit more work... Whether its worth it to ya or not i don't know...
Good luck!
Jesse
Last edited by sbcrx007 on Wed Jan 28, 2009 5:05 am; edited 1 time in total |
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| Posted:
Tue Jan 27, 2009 8:58 pm Post subject:
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Here's the file:
[/url]http://www.flyupload.com/?fid=424052804[url]
Well, I suck with web stuff, just cut and paste that ^  |
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| Posted:
Mon Feb 02, 2009 9:57 pm Post subject:
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SUPER!!!!
Very cool thanks!
What he could have done instead of the vinyl transfer (which is nice touch but probably expensive) is print each end on an 8.5 x 11 sheet at full scale, draw a reference line on each end of the template and define the length between the lines. Then you just print each template out on a regular printer, cut the paper and wrap around the tube ends. That's how all of my templates work btw. and NOW I will do the round tubes too! so cool.
Graber
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| Posted:
Tue Feb 03, 2009 10:12 am Post subject:
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That's another great idea! Good to know there's a better way for doing the round tubing. I think I'll stick with the reference lengths and paper as Steve is doing, but the vinyl is nifty.
I wonder what the difference is if you just build the frame originally with the slit profile? Obviously you wouldn't FEA that particular frame.
I haven't had a chance to play with the actual cutouts and tubing yet, does wall thickness make that much of an impact on the unfolded template? I was thinking that it would still match up to the real thing, even with actual wall thickness in, but I don't understand if solidworks compresses or stretches the metal as it bends it, or does both along the material's midplane? I just figured I'd play with that when I got to it.. |
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| Posted:
Tue Feb 03, 2009 10:35 am Post subject:
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| sbcrx007 wrote: | That's another great idea! Good to know there's a better way for doing the round tubing. I think I'll stick with the reference lengths and paper as Steve is doing, but the vinyl is nifty.
I wonder what the difference is if you just build the frame originally with the slit profile? Obviously you wouldn't FEA that particular frame.
I haven't had a chance to play with the actual cutouts and tubing yet, does wall thickness make that much of an impact on the unfolded template? I was thinking that it would still match up to the real thing, even with actual wall thickness in, but I don't understand if solidworks compresses or stretches the metal as it bends it, or does both along the material's midplane? I just figured I'd play with that when I got to it.. |
Good question about the unrolling. At our level of play such tolerances are probably within our margin of error anyways?
The physical tube you are cutting the profile needs to have the inner thickness ground down the match the shape of the mating tube. I also round down the pointy tips considerably to allow the miters to meet properly. As long as you don't grind the tube profile past the original marking of the template and allow your tube to mate flat against your other tube, the length will be spot on.
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| Posted:
Fri May 07, 2010 1:37 pm Post subject:
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hi, I know I am answering to an old post but..
this locost tutorial is mine, and I can just say that I have not noticed any dimensional problems with my frame... In a normal amateur workshop you can only measure to about +- 0.5 mm anyhow, so with a little care the frame turned out ok.
I have used the vinyl method as I am lazy and do not want to waste my time cutting paper stencils.. and much more importantly, I am working with vinyl all the time.... however, in a locost sense, it is expensive.. If you can find reasonable laser profiling for the tubing, that would be a much better idea.. I am sick of grinding the ends of tubing by now..
best regards
vlado
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