Question in Sketch 3

[JSMachine]

I am trying to figure out how to do something in sketch. Say I have a box. I draw the box in scketch, exit sketch, and then extrude it. I then take the solid (which is now a square), and start another sketch on one of the square's surfaces. On this surface sketch, I create a very detailed sketch with a lot of kines, arcs and points. I then exit scketch and do a cut only so deep, so it ends up being a pocket from the sketch I did.

After this, I flip the solid 180 degrees to the other side. I then start a sketch on that side (the opposite side of where I was working initially) and try to make a mirror image of what I did on the first side. When I exit the sketch, it too will be extruded and made into a pocket that matches the other side.

Now, what I would really like to be able to do is just somehow see the sketch from the other side, so I can simply trace it to the side I am working on. If I try this, it seems like I can only work in one sketch at a time, so therefore, none of my lines or points will snap to the sketch that is on the intial sketch. Sure, I could just redimension everything, but sometimes I am working with geometry that I have created off of the top of my head, and there is no real definition to it.

Is there a way to mirror the sketch to the opposite side I am working on?

Thanks!

 

[AnnaWood]

Read up on Convert Entities....

https://www.google.com/search?q=SolidWorks+Convert+Entities

Cheers,

Anna



Anna Wood
SW2013 SP4, Windows 7 x64

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[ctopher]

Per what Anna said.

View/Sketches
You can select the sketch from the Feature Tree also to convert its entities.

Chris
SolidWorks 13
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SolidWorks Legion

 

[JSMachine]

Awesome. That did the trick. Thanks agin folks.

 

[CorBlimeyLimey]

There is no need to retrace the sketch, or even convert it. Just mirror the pocket feature.

 

[mjcole]

Considering you wanted an exact copy of the feature on another face or you can do a derived sketch by ctrl selecting the original sketch and another face/plane.
Select Insert > Derived sketch. This will make an exact copy of your original that is fully defined except for location and orientation. The derived sketch will change whenever original is modified which requires less work to update your other duplicate sketches. The only restriction is that you cannot add additional entities to a derived sketch. You can also use a face pattern if it's not a thru cut. That's beyond the scope of your question though.

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[rollupswx]

or
Extrude your first sketch midplane.
Create your second sketch on the same plane (use origin planes as much as possible - they are the most stable) as the first.
Extrude-Cut Offset from the part surface to desired depth.
Show the second sketch and repeat on the other side.

Attach your *.sldprt file here if you can't figure out all of the three techniques suggested.