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Sheet Metal Model - Extrude - End Type Options

Anthony_SharpAnthony_Sharp Member Posts: 2
This may be on your to-do list already, but the lack of end type options in the "Sheet metal model - Extrude" feature is the biggest limitation I noticed when testing OnShape for potential use in our company.  The standard Extrude feature has Blind, Symmetric, Up to next, Up to face, Up to part, Up to vertex, and Through all options whereas the "Sheet metal model - Extrude" feature only has Blind and Symmetric.  Drawing a profile sketch and extruding is the fastest way to model a linear sheet metal part, and the lack of end type options makes it harder to use in a multi-part studio scenario where length needs to be based on other parts.  Especially when that studio will need dimensions adjusted or configured.


Thanks!

Comments

  • michael_mcclainmichael_mcclain Member Posts: 96 PRO
    You can put in an improvement request using the feedback tool. There may already be one, but I also agree that this functionality should be added in. It seems like something that should be present for adequate design intent of a model
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,464 PRO
    I agree. I'd like to see this too it makes sense to me that it should be the same as the standard extrude feature. 
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 823
    edited January 10
    Improvement requests are more useful submitted through the "Improvement Requests" section of this forum rather than the "Feedback" tool.  Feedback will log one ticket with us for yourself (and is useful for submitting bugs or questions), but posting an improvement request allows other users to vote on the request and also make their voice heard.  Each of those votes then adds another user ticket in our system and increases the priority of the request.
    Jake Rosenfeld - Modeling Team
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    @Anthony_Sharp
    @Jake_Rosenfeld
    @brucebartlett

    I have made a featurescript here based on the SM model feature that adds more extrude end type options.

    I have added "Up to face" and "Up to part" as options.

    Please give me feedback on the feature.
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    edited February 12
    @Jake_Rosenfeld
    @brucebartlett

    I have now added a "second direction" option.
    I have also added an option to offset from the face or part.

    A link to the new version is here:

    https://cad.onshape.com/documents/a39db7615a2a945ffb7076c3/v/ba3814b79b9f9de2f3e0df0e/e/dd6b70b441c40ff6bc4c8664

    Please send me feedback on this feature.

    Maybe this could be incorporated into the Onshape feature library.
  • lanalana Onshape Employees Posts: 265
    @mbartlett21
    Very nicely done. That is pretty much how we would do this. Thank you for doing this. It is interesting that you've added the second direction as well. Sheet metal Model menu is very busy. Do you think second direction option is sufficiently useful to justify  additional controls in that dialog? 
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,464 PRO
    lana said:
    @mbartlett21
    Very nicely done. That is pretty much how we would do this. Thank you for doing this. It is interesting that you've added the second direction as well. Sheet metal Model menu is very busy. Do you think second direction option is sufficiently useful to justify  additional controls in that dialog? 
    I think the second end condition could be useful.

    I also like to be able to select up to vertex, this is ideal for link to layout sketches
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    edited February 13
    @brucebartlett

    I could try to incorporate that into the feature.
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    brucebartlett said:

    I think the second end condition could be useful.
    It would be useful for offsetting from the sketch plane. That is what I would use it for.
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    edited February 13
    @brucebartlett

    I can't use up to vertex as it isn't supported by the opExtrude() function.

    I'll try to find a workaround.
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 1,365
    @mbartlett21 to do up to vertex, measure the distance and make the extrude blind. That's how it works in extrude.

    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • ilya_baranilya_baran Onshape Employees, Developers Posts: 775
    @lana
    I think the conclusion is that users want every conceivable option at once in a small, clean, and simple dialog  :)
    Ilya Baran \ Director of FeatureScript \ Onshape Inc
  • owen_sparksowen_sparks Member, Developers Posts: 1,295 PRO
    Also if you have a spare 5 minutes then you if you could move onto world peace, the moon on a stick and a stable version of windows then that'd be just awesome.

    Cheers, OwS.
    Production Engineer
    HWM-Water Ltd
  • lanalana Onshape Employees Posts: 265
    edited February 13
    mbartlett21 
    brucebartlett 
    Thank you for your response.

  • mbartlett21mbartlett21 Member Posts: 556 EDU
    @lana
    I would very much like it if you could have scrollbars in feature dialogue boxes, as well as indents.
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    NeilCooke said:
    @mbartlett21 to do up to vertex, measure the distance and make the extrude blind. That's how it works in extrude.

    @NeilCooke

    Actually, it does it in a slightly different way in the extrude() feature.

    It makes a plane and sets the end condition to "Up to surface".
    definition.endBoundEntity = createVertexBoundaryPlane(context, definition, vertexPlaneId);
    definition.endBound = BoundingType.UP_TO_SURFACE;
    Also, in the standard library documentation:
     <- Read
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 1,365
    Well, using blind is how I would do it  :)
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    @NeilCooke
    @lana
    @brucebartlett
    @Jake_Rosenfeld
    @Anthony_Sharp
    @owen_sparks
    @ilya_baran
    @michael_mcclain

    I have fixed a bug with the feature:
    When "Up to vertex" was selected, it created a plane at the vertex.
    I have also updated the FS version to 765.

    A link to the new version is here:
    https://cad.onshape.com/documents/a39db7615a2a945ffb7076c3/v/64ff265a8c16a316f2363426/
  • lanalana Onshape Employees Posts: 265
    Thank you @mbartlett21

  • mbartlett21mbartlett21 Member Posts: 556 EDU
    @lana

    How would I go about adding a manipulator at the other end of the extrude when i do a sheet metal model?
  • lanalana Onshape Employees Posts: 265
    Please check out extrudeManipulatorChange in extrude.fs , look for 

    SECOND_DEPTH_MANIPULATOR. You might be able to re-use extrudeManipulatorChange, it is exported 

  • mbartlett21mbartlett21 Member Posts: 556 EDU
    edited March 9
    @NeilCooke ;
    @lana ;
    @brucebartlett ;
    @Jake_Rosenfeld
    @Anthony_Sharp
    @owen_sparks
    @ilya_baran
    @michael_mcclain

    Bugfix released:
    When symmetric was chosen, the feature would not work correctly
    A link to the document is here: https://cad.onshape.com/documents/a39db7615a2a945ffb7076c3/
  • mbartlett21mbartlett21 Member Posts: 556 EDU
    Also if you have a spare 5 minutes then you if you could move onto world peace, the moon on a stick and a stable version of windows then that'd be just awesome.

    Cheers, OwS.
    @owen_sparks
    I am actually at school still, you know?
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,464 PRO
    Also if you have a spare 5 minutes then you if you could move onto world peace, the moon on a stick and a stable version of windows then that'd be just awesome.

    Cheers, OwS.
    @owen_sparks
    I am actually at school still, you know?
    Great work! Good to see you passionate about Onshape at a young age. You'd be the perfect candidate for an Onshape internship. 
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
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