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Laserkiste – a parametric finger joint box for laser cutting (stackable!)

florianflorian Member, OS Professional Posts: 110 ✭✭✭
edited November 2015 in Using Onshape
Hi Everyone,

based on those countless designs of simple boxes with finger joints I made my own. Why? Because I wanted a stackable version that scales as I need it. And sometimes you want to make adjustments that are quicker in Onshape than in a vector graphics tool.

The Onshape Document is called Laserkiste (German for Laserbox). Feature list:
  • Variables for inside length, width, height, material thickness
  • Variable for finger width
  • Finger count needs to be updated manually (They are calculated as #n_l, #n_h, #n_w , but linear patterns don't like variables yet)
  • Corners/Feet that are stackable
Ideas for the furture:
  • Take laser kerf into account => Booleans with "offset all" + extra Extrusion to make it 2D again
Have fun with it! And share your ideas on how to improve it.

PS: My favourite existing webtool: Makercase


Comments

  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,136 PRO
    @florian great work. I like the idea of building everything from the set of variables.

    florian said: Take laser kerf into account => Booleans with "offset all" + extra Extrusion to make it 2D againI love the boolean offset tool, works an absolute treat for projects like this. 
    What do you mean by "
    + extra Extrusion to make it 2D again"
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • florianflorian Member, OS Professional Posts: 110 ✭✭✭
    I love the boolean offset tool, works an absolute treat for projects like this. 
    What do you mean by "+ extra Extrusion to make it 2D again"
    I'm not sure. Just tried it. Here is an extreme version of the result. It should be a negative offset, but that results in a wrong geometry bad for a screenshot. I only want to offset the finger-faces while selecting them automatically. @brucebartlett, any idea?

  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,136 PRO
    edited November 2015
    Un check offset all, then do a window select from the side view to select faces that you require offset, if you select the window from bottom right to top left so it touch's only the face you want, I found this the quickest rather than selecting each face. I used the view cube to get a normal view to each face to do the window select. 

    You can also use Select other as shown in the pic below.



    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • florianflorian Member, OS Professional Posts: 110 ✭✭✭
    That's possbile, but it's manual?! I want to have it truly parametric and without manual changes. A parametric selection #feature would be a nice #improvement.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,136 PRO
    edited November 2015
    @florian, not sure how/if a parametric selection would work to select the side faces of the fingers as finger numbers vary.  

    The only way I can workout how to get it to work as fully parametric model would be to use the Boolean offset all, then to clean up the unwanted offsets with an extrude of the top face (by selecting the top face you will always get all the fingers), then another extrude of a sketched rectangle on the top face referencing the inside edges. Both to the thickness and merging to the top part. 


    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • florianflorian Member, OS Professional Posts: 110 ✭✭✭
    Here is a first example I made last week. Changes took me a few minutes (holes and #Arduino openings). I did not adjust for kerf (0.6 mm)=> The parts fit well when glued. Otherwise they fall apart.

    box.jpg 226.3K
  • jan_rychterjan_rychter Member Posts: 19
    Just stumbled upon this — thank you for creating this public example. I'm doing quite a bit of work with laser-cut designs as well.

    I encountered the same problem trying to adjust for laser kerf. "Offset All" isn't really applicable (because it offsets too many faces), and selecting individual faces is a *lot* of effort in a larger design.

    I am hoping OnShape will address this use case — anybody who laser-cuts designs will have the same problem.

  • jan_rychterjan_rychter Member Posts: 19
    @florian — I would also be interested in how you get from a 3D model in OnShape to vector files for the laser cutter. In SolidWorks, I used to create simplified drawings (without frames) that later needed some additional work (line thickness, colors, etc). Do you also use OnShape drawings?
  • florianflorian Member, OS Professional Posts: 110 ✭✭✭
    @florian Do you also use OnShape drawings?
    It's much easier than that! Select a face and right click! => Export as DXF.

  • jan_rychterjan_rychter Member Posts: 19
    edited December 2015
    @florian Thanks, this is great for small designs, for larger ones that you update it can quickly get problematic — but it'll work for now!
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    ....... trying to adjust for laser kerf. "Offset All" isn't really applicable (because it offsets too many faces), and selecting individual faces is a *lot* of effort in a larger design.
    .......

    There might be a way of addressing this which would also be very useful in the more general case. 

    Here's a selection idea for Onshape: Select a face, then choose "Propagate Selection", either directly from RMB, or perhaps as a subchoice within "Select Other". Then select an edge on that face to specify what direction to propagate selection, then roll the mouse wheel until the desired number of faces have been selected. During this process it would be possible, at any point, to "steer" the propagation in a new direction by picking a new edge on the last face selected. (The default edge adjoining the next face to be picked having been highlighted as each face was added to the selection set). If at any stage, the "wrong" next face is added, simply roll the mouse wheel in reverse to deselect it, then steer the selection by picking a different edge.

    The same functionality would be useful picking surfaces on Surface Bodies.

    In the meantime, it might be worth experimenting with the capability explained in this post by @lougallo, which is less controllable, but more powerful:

    https://forum.onshape.com/discussion/125/creating-selection-sets
  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,136 PRO
    edited December 2015
    I think we should start an improvement request for Tagging faces for DXF export. It would be ideally for this box, after changing the size 1 command to export all the required faces in 1 go. 
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • jan_rychterjan_rychter Member Posts: 19
    Just to clarify, the most important thing is for OnShape to remember the tagging somewhere. Even if it takes me half an hour to tag all faces that need to be exported, if OnShape can remember it for subsequent exports, it will be better than tagging everything each time I need to export.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    edited December 2015
    If this turns out not to be a priority for core Onshape, it might nevertheless be a capability a third party could usefully provide, using the API?
  • Marc_MillerMarc_Miller Member Posts: 110 ✭✭✭
    Very cool @florian, thank you for sharing this.

    I agree, being able to tag faces in some way for DXF export would be useful.
  • jan_rychterjan_rychter Member Posts: 19
    After doing some more experimenting and thinking, I do not think it makes sense to adjust for laser kerf explicitly in the 3D model.

    We are using a parametric modelling tool, so one typically models just a fraction of the entire assembly. You use a driving sketch, lots of mirroring, and then boolean operations to build the interlocking parts. It doesn't make sense to add offsets in the sketches, because they will get applied to both sides of your subtract operations. It doesn't make much sense to add them later (after the boolean ops), either, as it requires painstakingly selecting all the faces that need the compensation applied. And you still end up with an incorrect 3D model, where your parts intersect each other.

    Theoretically CAM tools are supposed to compensate for kerf, but it seems that in the laser-cutting world none of them do.

    What I would love to see in OnShape is slightly higher awareness of the laser cutting process. Tagging faces for DXF export is one thing, but let's take this further — at this stage we still have the full 3D model available, so OnShape knows what's "inside" and what's "outside" in the outline being exported. At this stage it is very easy to adjust for kerf — offset all the "outside" profiles with a positive value (make them effectively larger), and offset all the "inside" profiles (holes, basically) with a negative value (make them effectively smaller).

    Once OnShape exports to DXF, the inside/outside information is lost and can sometimes be hard to retrieve unambiguously.

    I would be very interested in taking a look at the API, but it doesn't seem publicly available? Perhaps with a little tagging support inside OnShape all the rest can be done externally?

    One thing I'd like to note is that if OnShape can nail this process, people who laser-cut 3D designs would love it immediately. There is no solution for this problem out there, just google for laser kerf compensation and see how much effort people expend on it in programs like CorelDraw, Inkscape, and others.

  • michael3424michael3424 Member Posts: 673 ✭✭✭✭

    One thing I'd like to note is that if OnShape can nail this process, people who laser-cut 3D designs would love it immediately. There is no solution for this problem out there, just google for laser kerf compensation and see how much effort people expend on it in programs like CorelDraw, Inkscape, and others.

    +1  I've no laser experience but will be getting one sometime next year and would really like to see @jan_rychter 's suggested features implemented.

  • florianflorian Member, OS Professional Posts: 110 ✭✭✭
    Theoretically CAM tools are supposed to compensate for kerf, but it seems that in the laser-cutting world none of them do.
    I guess that's true for those desktop cutters based on printer drivers. Those generally suck can be improved a lot. Don't worry, I have seen very small parts made with big production lasers (Trumpf). They compensate for kerf very well.

    summing up: kerf isn't a CAD but a CAM problem.

    Now I'm waiting for parametric linear sketch patterns and I'll be able to finish this document.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,136 PRO
    I would never model laser kerf into my model, I only would ever put in clearance's for ease of assembly and corner cut outs to allow for the small radius the machine will add in to the program. I with agree @florian that its up to the cam software and the laser programer to check for correct kerf compensation. I supply a drawings with critical sizes (with in reason) to be checked and assume the kerf would be adjusted if parts don't meet my spec. I do remember years ago getting some parts laser cut from wood and finding them to be quite loose when fitting together, it is most likely that when wood is cut it's hard to maintain tolerances as the laser burns the wood rather that with steel cutting with a molten kerf.


    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • jan_rychterjan_rychter Member Posts: 19
    @florian, @brucebartlett — We all agree that it would be nice to have CAM software that would do the job. But saying that will not make the problem go away. This nice laser box design is not going to be cut on big industrial production lasers. It's going to be used by hobbyists on (at best) Trotec cutters, and on Chinese 40W lasers most of the time. People who want the parts to match exactly will spend hours in CorelDraw or Inkscape manually offsetting outlines.

    Instead of waving the problem away, I was suggesting we think about how to improve things. After all, OnShape is supposed to be about rethinking CAD. So far my thinking led me to the conclusion that once you export the 2D DXF face outlines, you already lost information, and the CAM software has a much harder job, because you can't differentiate between product and waste. Which is why I was suggesting that instead of drawing a thick line between CAD and CAM, OnShape could accomodate some features which would make the process easier.

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭✭
    @jan_rychter

    I'm not sure that hobbyists are Onshape's target market.

    They're an important group for Onshape, certainly, because they may end up in a professional capacity as paying users (or that may be their day job), but essentially it seems to me that Onshape is primarily setting out to provide industrial-strength CAD for industrial users. You may have noticed they've strenuously avoided setting a hobbyist-level paid subscription offering.

    So it's not so much, perhaps, a question of waving the problem away, but of seeing that problem in the context of the core users of Onshape. It makes sense to me that they would focus the development resource on what's important to those users, and minimise adding capabilities (and the associated interface clutter) which would be extraneous for those users.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,136 PRO
    @jan_rychter you just need to master the offset command or offset boolean with the window select. 
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • show0kshow0k Member Posts: 1
    For those who fall on this thread looking for kerf compensation method for lasercutted parts, there is now a good FS : https//cad.onshape.com/documents/57df36a88f63301089e8ac78/v/17d807acd78c9661ab3cbd3c/e/157268905828b0fc910e365b
  • lemon1324lemon1324 Member, Developers Posts: 223 EDU
    Looks like your link isn't quite copied right.  For anyone landing here, here's the laser design suite of features I wrote:

    Kerf Compensation, T-Slot Joint, and Laser Joint.
    Arul Suresh
    PhD, Mechanical Engineering, Stanford University
  • michael3424michael3424 Member Posts: 673 ✭✭✭✭
    @lemon1324  - a very BIG thank you for creating those.  I've started making use of them for lasercutting and expect to be doing a lot more work in that area over the next year.  These Featurescripts will be a huge help on those projects.

  • MBartlett21MBartlett21 Member, OS Professional, Developers Posts: 2,031 EDU
    show0k said:
    For those who fall on this thread looking for kerf compensation method for lasercutted parts, there is now a good FS : https//cad.onshape.com/documents/57df36a88f63301089e8ac78/v/17d807acd78c9661ab3cbd3c/e/157268905828b0fc910e365b
    @show0k

    The link should have a colon (':') after the https at the start
    mb - draughtsman - also FS author: View FeatureScripts
    IR for AS/NZS 1100
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