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Is there a work-around for creating a pipe wrap-around template to cut mitered/contoured edges besides using sheet metal which squares edges off?

Question asked by Dave Krum on Mar 3, 2015
Latest reply on Mar 5, 2015 by John Stoltzfus

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Hello All,

Is there another possible way to develop a "wrap-around" paper template for cutting a pipe contour other than first converting the pipe to sheet metal, then choosing a k factor of 1 to get the correct outside flat pattern and plotting out the template full size? The problem with converting to sheet metal is that the software is changing the edges (as shown in the 2 screen snips 3 & 4) which is causing the overall length to be compromised (template too short now). I was thinking that maybe with the decal option (never used this) and choosing to cut it at the pipe edges with convert entities or something. Just throwing this out there. I will not get a perfect fit pipe if the shop guys use this template (will have to make one for each end due to length) and use pipe centerlines and match marks. I'm coming up alot shorter than I should, but the original pipe before converting to sheet metal is right on the money. Captures 1 & 2 are shown with the pipe. Captures 3 & 4 are shown using sheet metal. Capture 5 is the flat pattern but uses the sheet metal which makes the edges square (normal cut since its sheet metal) and thus shorter of what the template should be. Thanks in advance.

Attaching the part file and "saved body" file as well showing just the pipe after I converted to sheet metal.

John Stoltzfus Mar 4, 2015 1:10 PM

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I'm from the old school when it comes to sheet metal - everyone (or it seems) is on to multi body sheet metal, might be ok, but like I said "Old School", lol The way I would approach a project like you showed was to place the flanges and determine the pipe center line, draw two equal lines and in the center between the two I would have added a plane and that is where my pipe sketch would have been, then I would have extruded up to each flange and that would have automatically given me the end cuts. The sketch would have been a semi circle, where you leave just a little slit so you can add the sheet metal feature, then for what you need, I would have made 2 configurations..

Either way works, some might be slower or more robust or better or worse, really doesn't matter, find your comfort zone and go from there

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John Stoltzfus Mar 3, 2015 3:50 PM
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Dave,

Change your material thickness to .001 and see what happens in your flat pattern - What I would do is make one the thickness you need in your model as one configuration and the thin pc just for a pattern that your asking for in another configuration.

I had done a lot of pipe cuts like that and they are normally right on.
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- Dave Krum @ John Stoltzfus on Mar 3, 2015 3:52 PM
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  Hi again John! 12 std. pipe has a .375 thick wall and that is what its set for. I don't believe I can change the sheet metal can I? I did change the radius to .001 (but don't think this matters for a round) and the K to 1 but the thickness is grayed out.
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  - John Stoltzfus @ Dave Krum on Mar 3, 2015 3:56 PM
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    I think you should be able to add a configuration -
    
    If not I would do a save as a copy and open that file - it doesn't have to be .001 - even .015 will get you where you need
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- Dave Krum @ John Stoltzfus on Mar 3, 2015 3:57 PM
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  Ddn't see the rest of your reply. I can try making 2 configurations but how do I change the thickness? I'd have to change the profile right after I created my 3d line I think.
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  - John Stoltzfus @ Dave Krum on Mar 3, 2015 4:12 PM
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    Dave you should be able to change your metal thickness on the sheet metal - can you post a screen shot of your feature tree expanded
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    - Dave Krum @ John Stoltzfus on Mar 4, 2015 5:43 AM
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      John,
      Here is the FMT expanded (shows thickness as .375 under equations and I cannot change it under sheet metal - its grayed out). I did post the .sldprt file yesterday. I'm thinking because I used structural member to create the pipe profile (in lieu of sketching the cross section profile) that I am not allowed to change the thickness. If I change from structural member for the pipe to a sketched profile, then it may work but I think I would need to start over with my trims to plate etc. I've been using SW for over 2 years, but this is the first time I'm attempting to use it for developing pipe templates so please be patient lol. Thanks.
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      - John Stoltzfus @ Dave Krum on Mar 4, 2015 6:49 AM
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        Dave
        
        You can make another pipe part but keep the thickness very thin to get a better flat pattern - I would be a little cautious with that, because SW is pretty good with flat patterns on skewed pipe - the thinner you go the longer the pc will be.
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        Dave Krum @ John Stoltzfus on Mar 4, 2015 7:06 AM
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        Hi John,
        You're saying to make another profile to set up as a structural member, just with the thin .01 wall or so? That is probably the reason why I can't change the thickness, cuz I used structural member for the pipe? I'll make a new profile as structural member, then set up 2 configurations, one for the normal pipe thickness, then a new one for .01 thickness.
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        John Stoltzfus @ Dave Krum on Mar 4, 2015 7:34 AM
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        That should work for ya
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        Dave Krum @ John Stoltzfus on Mar 4, 2015 12:41 PM
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        John,
        I tried making a profile file of the thinner pipe wall (.01") as we discussed so I can use the "structural member" option to choose my pipe sizes. I was gonna use both the 12 std. pipe (12.75 o.d.) and the new profile for the template with 12.75 o.d. and .01" thickness. When I go back to the model, I was hoping I could set up the structural member profile under configuration, choosing each accordingly but apparently the option to choose configurations for the structural member profile wasn't added to a later version and I'm still on SW2010. So as a workaround, I just sketched in the o.d. profile and used the thin feature to extrude. Then for the thickness of the thin feature, I configured it for 2 configs, one for the original thickness and one for the template. This seems to be working! Good idea. My template is coming out within a 1/32" when I use the K factor of 1. Thanks again.
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        John Stoltzfus @ Dave Krum on Mar 4, 2015 12:47 PM
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        Glad it worked for you, the next time I would model the pipe and add a slit cut and insert the bends after the end cuts. That way you can very easily add a configuration and change the dimension for the thickness value
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        Dave Krum @ John Stoltzfus on Mar 4, 2015 12:58 PM
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        Yeah, good idea. I added the new configuration to the original model file (the new one being for the template but I didn't slit it at this time). Then used "save bodies" to save just the pipe to another file. From that new file (which already has both configurations), I activated the template config then slit the pipe and converted it to sheet metal. Do you do all of this right from the original model file without creating a new file with just the one body? Sounds like you do alot of the same thing that I do, so I value your expert opinion. Cya.
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        John Stoltzfus @ Dave Krum on Mar 4, 2015 1:10 PM
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        I'm from the old school when it comes to sheet metal - everyone (or it seems) is on to multi body sheet metal, might be ok, but like I said "Old School", lol The way I would approach a project like you showed was to place the flanges and determine the pipe center line, draw two equal lines and in the center between the two I would have added a plane and that is where my pipe sketch would have been, then I would have extruded up to each flange and that would have automatically given me the end cuts. The sketch would have been a semi circle, where you leave just a little slit so you can add the sheet metal feature, then for what you need, I would have made 2 configurations..
        
        Either way works, some might be slower or more robust or better or worse, really doesn't matter, find your comfort zone and go from there
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        Dave Krum @ John Stoltzfus on Mar 5, 2015 6:59 AM
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        Thanks for your advice John. I sketched my two plates first on the top and front planes. Then sketched in a 3d line on the skew from the front plane where the pipe starts. Then drew the circle on edge of 3d line and extruded outward in both directions. Then set up planes and cut pipes with "cut with surface". I tried extruding it "up to next" on the plate side but with the cutouts in the plates, I was getting some weird error. So I just went far out in both directions and cut it to the miters using planes I set up. And then of the procedure was pretty much based on what you suggested. I plotted out the template from the sheet metal config. The shop is gonna try it out today and see how it pans out. My flat on the 360 roll and overall length looks pretty darn good.
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        John Stoltzfus @ Dave Krum on Mar 5, 2015 7:25 AM
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        Thanks for the update
        
        Hope it works well, and have fun
        
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