What is the best way to define a sketch that is cut and pasted to a new sketch?

john_eisenlohr500

I copied sketch # 4 from this sketch - https://cad.onshape.com/documents/4465c5faccd7343b7e1964c8/w/5e06206945f9ce14f0ebd24d/e/5993bf2281242f431cff8875
and pasted it on this sketch - https://cad.onshape.com/documents/261ab941428be6d7a961009f/w/f6723fab072258fb93d8bd4a/e/82b6bb894412f9fa1eee1ee9
What is the best way to get it defined on the new sketch?

MichaelPascoe

Hi @john_eisenlohr500, here are some techniques I use all the time for projects like this one:

Sketching best practices:

• Minimize dimensions and constraints to external references. For example, do not dimension to the origin, instead, draw a construction circle within that same sketch and dimension things to that. Then, constrain the construction circle to the external reference if needed. This way when you copy and paste, all of the dimensions are good and you only need to constrain the construction circle.
• Use an implicit mate connector to place the origin of the sketch instead of using a plane. This will let you easily reposition the sketch however you like without breaking the constraints. It also gives you more control over the orientation of the sketch.
• Fully define your sketch with dimensions and constraints. This way when you move the sketch, everything stays how you intended.
• If you do need to dimension or constrain to external references, be very intentional with where you dimension or constrain to. Poor placement of dimensions and constraints can lead to failed sketches when the model is changed. Dimensioning to faces is more robust than edges and points. Dimensioning to original sketches can sometimes be better than dimensioning to a part.
• If the sketch was imported from a dxf, you may need to re-draw it using dimension-able shapes from within the Onshape sketch.

https://cad.onshape.com/documents/f6a2770b506108d1a2cf9b9e/w/cf182fdfa5f9bbf1d5bc3e80/e/8a867b4dcafa98faa95f4e4a?renderMode=0&uiState=63f4bc9d51ceb127feb88718

john_eisenlohr500

I tried to follow what you did but its not working. I can't lock the construction circle into my existing sketch. The circle has no center point like your sketch.  https://cad.onshape.com/documents/4465c5faccd7343b7e1964c8/w/5e06206945f9ce14f0ebd24d/e/5993bf2281242f431cff8875
 
I'm assuming the pasted sketch has to be lined up perfectly with the origin to be defined. I can get it close to the origin with the transform tool but it's always slightly off.   https://cad.onshape.com/documents/c46f665af826677a2066fe01/w/8ad22d913b81cf935616cf22/e/ff54f937d00075ca005ea44a 

  Since that doesn't work I tried the coincident command. I can get it on the origin but its not defined. https://cad.onshape.com/documents/c46f665af826677a2066fe01/w/8ad22d913b81cf935616cf22/e/ff54f937d00075ca005ea44a

MichaelPascoe

I've never seen a construction circle without a center point. Which sketch has the construction circle?

The pasted sketch does not need to be lined up, that is the neat thing about this technique; everything should dimensioned or constrained relative to the construction circle. This way you can constrain the construction circle to the other sketches without any trouble.

The sketch must be fully defined relative to the construction circle. Then you can constrain the construction circle to whatever you want. I constrained it to the implicit mate connector for easy orientation of the sketch.

If the sketch constraints are still giving you trouble, check out the learning pathways in the learning center, its pretty legit and has saved me tons of headaches. Specifically, this course should help: Learning Center - Introduction to Sketching

S1mon

A few tricks might help with this process:

1. Using the transform tool is a quick way to grab all the elements of a sketch, move it slightly and remove any constraints which are tied to the origin or any other reference geometry.
2. If you temporarily fix the point you want to use as a reference (it doesn't have to be the center of a construction circle, I would normally use an end point of a line, or a sketch point aligned to a midpoint or whatever), everything should turn black (be fully constrained). Depending on the constraints you added to your sketch, you might need to constrain something horizontal or vertical.
3. After you've confirmed that locating the sketch (the fix, plus optional horizontal or vertical) works, then you can copy and paste with confidence that you'll get the same thing each time.