Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:

  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

tube cutting for weldments

glen_dewsburyglen_dewsbury Member, OS Professional Posts: 119 PRO

I have a problem that overlaps a question about how to and what I see as an error. I plan to post this on the forum as well to see if anyone else has run into the same concern and may have an answer.

I’m fitting tubes together for a weldment. Initially leaving supplier to take care of trimming tube ends since that is what they do to manufacture parts for us. The supplier cuts tubes using a machine that takes my extruded parts and cuts normal to the part axis which eliminates feathered edges that don’t work well for welding. We want to do this operation ourselves to save some time. I have not been able to work out the means. Tried a remove swept profile but the tracking has to change from outer to inner curve. My difficulty is determining where that transition has to happen so I can use 2 curves with a sweep remove.

Also tried using sheet metal parts since they have a normal cut as I need. The sheet metal tool doesn’t seem to know any better than me where the transition from inner to outer is and just follows the outer edge. The attached file has an example. It leaves material that produces interference fit. Also as shown on example is a cut where a secondary tube has to fit over primary. In sample provided it mostly works but leaves residual ‘parts’ not wanted. Some of the trimming of secondary cut out works but gives an error on about 50%. I don’t know why and no messages indicating what’s wrong.

Am thinking to provide paper flat layouts to our shop during development to save time by providing a wrap around template for tube cuts.This would require accurate flat patterns not always available when errors occur. Getting a flat pattern suitably sized for the diameter as a wrap around is no trouble when K facture of 1 is used.

Best Answer

Answers

  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 2,537
    Hi Glen, this is similar to this discussion https://forum.onshape.com/discussion/comment/48596#Comment_48596 however, I will take a look at this in more detail tomorrow.
  • glen_dewsburyglen_dewsbury Member, OS Professional Posts: 119 PRO
    edited May 31
    Looks like I got it in the sheet metal version. Have to play with the spline used to trim flat pattern for accuracy.
    https://cad.onshape.com/documents/c45db00a5a31d0922777e376/w/e78ad8cc56aa30565126205e/e/a45f4ac1b3d9f987ce586a91
    A tool path as used in Solid Works would be a lot less tedious. I think there is an IR for tool path.
    Would prefer OS sheet metal to work a little better for determining end conditions.
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 2,537
    Interesting problem - even a toolpath would not help as the point of intersection moves from the ID to the OD when the pipe is at an angle? Sheet metal should get it I suppose if we could create a fully closed pipe. Not even sure how to do it in FeatureScript.
  • MBartlett21MBartlett21 Member Posts: 1,666 EDU
    @glen_dewsbury
    You should be able to boolean the part named "Stub w/ no cut outs" from the sheet metal tube and it should cut it correctly
    MB - I make FeatureScripts:View FeatureScripts
  • glen_dewsburyglen_dewsbury Member, OS Professional Posts: 119 PRO
    Thanks for the idea MBarlet. Just tried it and no change to SM part. Seems that it should work but boolean comes up red. A SM limitation I believe.

    There are two directions I'm working from Neil.
    Standard production would use extrude that needs to be trimmed to match what the cutting machine produces.
    If I could manage to find the change over points (which is what I'm trying to do now) then 2 sweep removes starting and ending at the change over would do the trick.
    The second for prototyping where SM works to provide a wrap around paper template. This reduces time to completion as we no longer need to involve an outside vendor. Trimming in the flat is quite tedious when there are a number of pieces but may allow for FS automation once I get the specific details worked out better.
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    coping with this.......

    I've built mountain bike frames from hydro formed parts.

    -each bike frame style had it's own partstudio, keep it simple
    -the sizes were controlled by configurations
    -there was a layout sketch controlling top, down, seat, chain stays, rake & offset
    -positioned tubes to sketches
    -coped tubes with surfaces, did not use booleans


    Anyway, the fabricator became a really good friend of mine. Our welds were minimal because the tubes fit. There wasn't any weld filling going on with my frames. They looked really good.

    My deliverable was one 1:1 drawing that they printed out and sandwiched between some plexiglass for the welders. This one fixture drawing had everything on it to make a bike frame.



    I was controlling 5 or 6 different styles of bikes, I don't remember how many frames for sure, there were several.



  • lanalana Onshape Employees Posts: 488
    @glen_dewsbury
    How about this https://cad.onshape.com/documents/a89c5cafab733cc817ab2463/w/23e10c658be967f990d7a708/e/55c16516b9f7dbd7a7937c81 ?
    I've merged solid cylinders and flipped thicken direction in sheet metal.
  • bryan_lagrangebryan_lagrange Member Posts: 258 ✭✭✭
    I used to work at a facility that had a Trumpf tube laser. We created square, rectangle, and round tube in sheet metal to get the normal cutouts and flat  pattern which at the time Tops 400 (CAM software) needed. 

    Here are some guidelines I used. 
    1) To get the most accurate flatten state of the tube I always set the K factor to 1
    2) Measure and use the thickness of the tube (round, square,and rectangle) and input as thickness in sheet metal
    3) For rounds I would make a circle then cutout .005 degree section.
    4) For rectangle and square tube measure the inside radius of the corners and draw them in. Use  .001" thickness cut (or smallest that the software will allow and make a flat pattern). Place cut in one of the faces of the 

    https://cad.onshape.com/documents/3e2e44b75c451dddaf3dfcd4/w/92eb30a1ec9d776b564aec26/e/d35344de636647951abc82ed
    Bryan Lagrange
    Twitter: @BryanLAGdesign

  • steve_shubinsteve_shubin Member Posts: 101 ✭✭✭

    This is my first time posting, so I hope I didn’t do anything wrong

    As per EricGauthier instructions, I used Thicken with Intersect

    I did not use any sheetmetal tools

    I did not deal with adjusting any splines

    THERE IS QUITE A DIFFERENCE between glen_dewsbury SHEETMETAL METHOD and the THICKEN WITH INTERSECT METHOD on 2 of the parts

    Funny thing is, there appears to be no difference between the two methods on what Glen called the REGULAR TUBE

    The parts made with the SHEETMETAL METHOD are all colored GRAY.

    The parts made with the THICKEN WITH INTERSECT METHOD are YELLOW, ORANGE, and GREEN colored

    I didn’t move anything. I brought in all the sheetmetal parts using DERIVED

    Go take a look at the Named View that is called Closeup

    Turn on the 2” tube, and then turn off tubes 1, 2, and 3 — the sheetmetal tubes. Look how the thickened tubes (yellow, orange, and green) fit against the 2” tube

    I don’t have the URL for my document as I only use Onshape on my iPhone and never see the URL. But, I can give you the name of my document and you can search for it by name

    tube test juxtaposed

  • steve_shubinsteve_shubin Member Posts: 101 ✭✭✭

    This is my first time posting, so I hope I didn’t do anything wrong

    As per EricGauthier instructions, I used Thicken with Intersect

    I did not use any sheetmetal tools

    I did not deal with adjusting any splines

    THERE IS QUITE A DIFFERENCE between glen_dewsbury SHEETMETAL METHOD and the THICKEN WITH INTERSECT METHOD on 2 of the parts

    Funny thing is, there appears to be no difference between the two methods on what Glen called the REGULAR TUBE

    The parts made with the SHEETMETAL METHOD are all colored GRAY.

    The parts made with the THICKEN WITH INTERSECT METHOD are YELLOW, ORANGE, and GREEN colored

    I didn’t move anything. I brought in all the sheetmetal parts using DERIVED

    Go take a look at the Named View that is called Closeup

    Turn on the 2” tube, and then turn off tubes 1, 2, and 3 — the sheetmetal tubes. Look how the thickened tubes (yellow, orange, and green) fit against the 2” tube

    I don’t have the URL for my document as I only use Onshape on my iPhone and never see the URL. But, I can give you the name of my document and you can search for it by name

    tube test juxtaposed

  • john_mcclaryjohn_mcclary Member, Developers Posts: 2,108 PRO
    edited June 2
    @steve_shubin
    Welcome to Onshape and the forums!

    You can get a link by clicking the copy link button
    under the share area

  • glen_dewsburyglen_dewsbury Member, OS Professional Posts: 119 PRO
    edited June 2
    It's getting closer to a complete answer.
    I started out working the way Brian Lagrane describes the process. Seamed like a rational approach right from the beginning. Gave me what I was looking for except interference fits.
    Try my part studio 4 and have a look at what happens when all tubes are the same diameter. Which I do need to deal with.
    Some times fails on secondary cuts as well. Not always. Have not been able to determine why.
    Seams I still have the same failures when tube sizes are the same. Intersections are not understood so well by OS.
    Remnants left behind that are showing up in the flat pattern as well as the model.
    When I make all tubes the same size all heck breaks loose.
    The other methods suggested leave me with interference between parts which I had seen before. That's what got me trying to do secondary trimming in the flat pattern. Not a good way to do things I agree and very time consuming.
  • glen_dewsburyglen_dewsbury Member, OS Professional Posts: 119 PRO
    edited June 2

    all in part studio 4.
    Tried set up with tubes at 3" 2" 1" and things seemed to work pretty good with only a couple remnants that I could deal with.
    Changing the position of the gap seemed to have some positive affect.
    Tried various tube sizing keeping the ratio the same and could continue.
    When I added a matching hole in the central tube I was left with some notable gaps.
    Changed to all same size even with the O/S offset for cutouts and well ........
    I'm thinking this is something for OS to deal with in future updates.
    Thanks for the help Bryan.
  • bryan_lagrangebryan_lagrange Member Posts: 258 ✭✭✭
    @glen_dewsbury I also use to do slot and tabs to help locate pipe pieces together when we would cut the pipe on a CNC laser. It has been a while since I did this but I added them to the model to give you an idea. Along with slot and tab I used to etch text at connection points (Examples at a slot I would put A1 and the corresponding tab I would etch A1) to help speed up the fit up during fabrication.


    Bryan Lagrange
    Twitter: @BryanLAGdesign

  • steve_shubinsteve_shubin Member Posts: 101 ✭✭✭

    @john_mcclary — Thank you for the welcome John

    It looks like my free (hobbyist) version of Onshape does not have that capability to — Copy link to clipboard


  • john_mcclaryjohn_mcclary Member, Developers Posts: 2,108 PRO
    edited June 3
    Or it could be an IPhone thing.. odd, usually the iPhone gets features first with the app.

    Another trick is to open a web browser and copy it from there. Even though you can't do much with the model, you can still do some tasks with mobile browsers. Like copy your link, edit featurescript, etc.
  • steve_shubinsteve_shubin Member Posts: 101 ✭✭✭
    @john_mcclary
    It’s only been a few times that I’ve seen an Onshape document through the iPhone Safari browser. And I just can’t figure out how to get back to there and do that again.
  • steve_shubinsteve_shubin Member Posts: 101 ✭✭✭

    The thought struck me that it’s possible the different browsers and platforms they run on, may handle graphics at least a little bit differently with regards to Onshape. So I thought I better post a picture of the DIFFERENCE that I’m seeing between the SHEETMETAL METHOD and the THICKEN WITH INTERSECTION METHOD

    In short, the sheet-metal parts are shown in gray. And the green and orange parts are that of the thicken with intersection method 

    For a better description of all this, you could read my original post up above


  • john_mcclaryjohn_mcclary Member, Developers Posts: 2,108 PRO
    Goto cad.onshape.com  then login 
  • glen_dewsburyglen_dewsbury Member, OS Professional Posts: 119 PRO
    I like the tab and slot locating. Was asked for that not long ago and it worked quite well.
Sign In or Register to comment.