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.

Using 'Use' and Possible Alternatives....

larry_haweslarry_hawes Member Posts: 411 PRO
edited April 30 in Using Onshape
I tend to use the 'Use' command a lot to duplicate earlier sketches but then, very often, want to modify the second sketch which requires deleting many many Use constraints before proceeding with the modifications. Is there another way to 'use' a previous sketch as the basis for another sketch without the 'Use' command? Or is it just a difficult task when using this method?

Thank you 



https://cad.onshape.com/documents/c7ac382255c4440e75bf4ef3/w/1f3e5ec88beba41434f1492d/e/4acce76f9471456354ecfedd

Best Answer

Answers

  • MBartlett21MBartlett21 Member Posts: 1,622 EDU
    You can copy and paste sketch entities between sketches.
    MB - I make FeatureScripts: view FS (My FS's have "Official" beside them)
  • larry_haweslarry_hawes Member Posts: 411 PRO
    edited April 30
    Can that be done and position the copied sketch in the exact location as the previous sketch? Seems to place the copy randomly? I have another software program that has a paste/hold position command to place objects in the same position as the copied entity. Is there such a feature in OnShape
  • Cris_BowersCris_Bowers Member Posts: 281 PRO
    There are several workflows you can use, and I think consideration needs to be taken into what you are trying to accomplish. Are the cutouts in the parts supposed to be the same size? If so, you can extrude the cutout through both parts without having to recreate or use the sketch. Is the cutout in the top part supposed to be the same shape but larger? You can still create the cutout through both parts then use the "move face" command to offset the faces of the cutout in the top part. Is it a similar but different shape? Then you are probably better off copying or redrawing the sketch and modifying the dimensions. Also do your parts lend themselves to configurations? In your example the parts look to be almost the exact same profile, one is just rotated 90 degrees. This might be a case where you create 1 part and modify the dimensions for different configurations.

  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 2,396
    Hey @larry_hawes - I think it depends on the final shape you are after - just offsets? different entity types (lines -> arcs)? One thing you could do is keep the used sketch entities and then offset the ones you want to offset using the offset command ( :) ) - you would then have to close the gaps between the offset entities and the used entities and select all the regions while extruding (or convert the used entities to construction). Or you could extrude and use Move Face, or you could...
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • larry_haweslarry_hawes Member Posts: 411 PRO
    There are several workflows you can use, and I think consideration needs to be taken into what you are trying to accomplish. Are the cutouts in the parts supposed to be the same size? If so, you can extrude the cutout through both parts without having to recreate or use the sketch. Is the cutout in the top part supposed to be the same shape but larger? You can still create the cutout through both parts then use the "move face" command to offset the faces of the cutout in the top part. Is it a similar but different shape? Then you are probably better off copying or redrawing the sketch and modifying the dimensions. Also do your parts lend themselves to configurations? In your example the parts look to be almost the exact same profile, one is just rotated 90 degrees. This might be a case where you create 1 part and modify the dimensions for different configurations.

    Thanks Chris, The model I posted was as simple as I could make the example and my needs have varied in the past. The 'Use' command works very well but am looking for an alternative and I think similar but different is a good description of the challenges of past models. Didn't think about configs. 
  • larry_haweslarry_hawes Member Posts: 411 PRO
    edited April 30
    You can't paste it in the same location, but it will retain all "internal" constraints, including dimensions, constraints etc. That means that you can pretty easily constrain the newly-pasted sketch to your original sketch (and depending on how many "external" constraints are required, it could be very simple). This way you can retain your design intent in the new sketch, but easily put it in the right location.

    You can use Coincident between the new sketch entities and the old ones...this at lease will give you only 1 constraint to change per line (as you know, the "Use" command produces 3 constraints: the line, and the vertices at each end of the line).

    Good luck!
    Romeo
    Interesting approach, and seems like it might serve the purpose best. Don't think I've constrained a sketch to a previous sketch before but if I use coincident between sketches this could allow the copied sketch to be placed in the same location as the original. I'll try it on my simple model. Thank you

    This worked pretty well and will give me another option as well as the other ideas posted.

    Thanks for all the help...
  • larry_haweslarry_hawes Member Posts: 411 PRO
    NeilCooke said:
    Hey @larry_hawes - I think it depends on the final shape you are after - just offsets? different entity types (lines -> arcs)? One thing you could do is keep the used sketch entities and then offset the ones you want to offset using the offset command ( :) ) - you would then have to close the gaps between the offset entities and the used entities and select all the regions while extruding (or convert the used entities to construction). Or you could extrude and use Move Face, or you could...
    Thanks Neil, The final shapes have varied in the past from simple offsets to different entity types (lines->arcs) and again the Use command works very well but...convert the used entities to construction...hmmm. Interesting idea thanks again. 
Sign In or Register to comment.