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Scaling Sketch

dennis_tangdennis_tang Member Posts: 5
I am looking to see if there is a way to scale a sketch.  I copied a sketch but i would like to scale down in size. Is the a way in doing so?

Answers

  • hans_van_de_burgthans_van_de_burgt Member Posts: 3 EDU
    Same question...
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,387 PRO
    There is no direct 'sketch scale' feature currently available. There are few workarounds for occassional scaling though:
    - Simple sketch might scale with sketch offset
    - If there is only one dimension driving, sketch will scale automatically according to that
    - By using variables you could create multiplier to change scale of all dimensions
    - Ultimate solution is to create dummy part with original sketch shape, scale part, create another sketch and use/project part edges, then hide/remove body
    //rami
  • alex_ryanalex_ryan Member Posts: 6 PRO
    easiest way is to create a scale factor with the first entity you dimension.  i'll draw a line in my sketch at like 1", then dimension that to whatever i need.  long as it's the first dimension it'll scale the whole sketch for you.  
  • viruviru Member, Developers Posts: 619 ✭✭✭✭
    edited October 2016
    @dennis_tang, Currently scaling of sketch is not available in Onshape. You can raise improvement request for this. In near future we hope that this facility will be provided by Onshape. Till time you You can use below work around for this issue.
    create relationship for dimension by using variable feature. Kindly refer below video which will be helpful in dimension creation by using variable.





  • biscuitladbiscuitlad Member Posts: 8
    Did this get anywhere? The problem for the work arounds is that they don't work for lofts. When creating a series of spline profiles, it would be very convenient to be able to project a profile onto an offset plane and then scale that profile down or up to create tapered forms. There is no way of doing this at the moment.  
  • paul_chastellpaul_chastell Onshape Employees Posts: 116
    @biscuitlad, There's a bunch to explain here. First off, how does scaling work today? When you change a length dimension (distance, radius, diameter) Onshape will look to see if the sketch can be scaled without violating any of the constraints that are there or any of the other dimensions. Obviously having two different length dimensions will cause Onshape not to scale but also having more than a couple of external references will also do that. On the other hand Onshape understands that angle dimensions don't care about a sketch scaling and so you can have angle dimensions and scaling will still work. If you have multiple length dimensions you can set some driven before the scale and then set them driving after.

    When you project a spline onto a new sketch what you get is a spline that cannot be deformed, only moved and scaled. At the same time (because you said to project it) you get constraints to lock it to the parent spline. As a result when you add dimensions to that sketch it knows it can't scale without violating those constraints. The way to get this to work, therefore, is to delete the constraints, one on the spline and one on each end point and then add a dimension and change it to scale the sketch. 

    Your particular example may not be as simple as that but here is an example I just threw together with three copies of splines, all scaled using dimensions and making a tapered loft. I seem to have made a start on a possibly uncomfortable bike saddle.

    https://cad.onshape.com/documents/be8d97b063ffe48b53625dd3/w/9c70f222e1c6d18075d3ab79/e/5cbde84e4b955d34a2678a38

    I'm not saying the need for a function to do this wouldn't be useful or that we will never have one, but it should be possible to follow the same steps manually that a dedicated command would do.

    Note: doing this means the 'child' is no longer going to change if the 'parent' does, which would happen if the constraints were still there. However, this wouldn't be any different if we had a dedicated scale function. If you wanted to have scaled splines that are related to each other I would suggest sketching separate splines with distance dimensions pinning down the locations and variables specifying the dimensions that are used across the sketches. See the other element in that document for an example that has scaled splines. I did it by copying the original sketch onto the different planes.

    https://cad.onshape.com/documents/be8d97b063ffe48b53625dd3/w/9c70f222e1c6d18075d3ab79/e/4a22c0c5541ee3ac6b4f52f4
    Paul Chastell / VP of R&D / Onshape Inc.
  • Auke_SmitAuke_Smit Member Posts: 14 PRO
    Is the scaling sketch function upcoming? 
    I import dxf designs some times, and then I want to be able to scale the lines, without having to dimension all lines, (or editing the original file)

    Work arround of extruding and then scaling works for me, but scaling the sketch seems cleaner.


    Even grouping sketch entities would be great in my case. So I can make a rectangular box arround it, group it, so all internal relations are fixed, and then dimension an edge. 
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,297 PRO
    Why can't you just project a curve, make it construction, then offset that curve?

    Seems like it would be easy to understand. Is an offset equivalent to a scale? It's too early in the morning, but I'm going to say yes. 


  • steve_shubinsteve_shubin Member Posts: 57 ✭✭
    edited August 6
    @Auke_Smit

    As to the first paragraph of your post above ———

    I imported a DXF

    I scaled it by placing one dimension

    I deleted that dimension

    I placed another dimension and scaled it a second time



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