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A cad software is only as good as the basic sketching is
tore_thoresen
Member Posts: 4 ✭
...or am I missing out on something?
I cannot find that it's possible to snap along an edge, corner, midpoint or anything else on an extruded model when sketching on a face.
Also when you are transforming some line or anything on a sketch, snapping doesn't seems to work.
I cannot find that it's possible to snap along an edge, corner, midpoint or anything else on an extruded model when sketching on a face.
Also when you are transforming some line or anything on a sketch, snapping doesn't seems to work.
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3dcad
Member, OS Professional, Mentor Posts: 2,470 PRO
It's difficult to say anything without seeing the actual model but if you can't snap onto existing geometry then you can click 'use/project' command and bring those edges into current sketch. Hit construct before use to make them constrution geometry.
I agree with the title and that makes Onshape pretty awesome piece of software.
//rami5 -
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lougallo
Member, Moderator, Onshape Employees, Developers Posts: 2,001 
If the face is shared with the sketch plane we do inference those entities. What browser are you using?Lou Gallo / PD/UX - Support - Community / Onshape, Inc.5 -
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chris_8
OS Professional Posts: 102 PRO
I agree OS sketching lacks in usable "live" points from background sketches or other entities. You can make a point, then tell that point to be coincident with a corner from something in the background, then use that new point to start a line. But you can't simply compress all these tedious steps by starting a line at the corner of something in the background.
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Options3dcad
Member, OS Professional, Mentor Posts: 2,470 PRO
It can be also good thing if you have a lot of background stuff.
I have often cases where new line begins 1mm from something in the back, I hate when cad tries to be smarter than me and snap onto things I don't want.
But we do have shift -function to disable snapping so we could also have button to wake up everything in background?//rami5 -
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brian_brady
Member, Developers Posts: 505 EDU
When I tech Creo that is a common complaint from students who have used SolidWorks or other 3D CAD applications. In Creo, you have to add references for any existing geometry that you want to snap to but not with all other packages. All other geometry is ignored. Once a model gets complicated, I personally appreciate that all geometry does not cause the cursor to snap on something that is meaningless to what I am working on. In Onshape, you have to either project points, edges or intersects for snapping. This is okay, but I don't always want edges to become lines or curves that will have to be trimmed, I just want to reference those lines or curves. Making them construction features works okay.chris_8 said:I agree OS sketching lacks in usable "live" points from background sketches or other entities. You can make a point, then tell that point to be coincident with a corner from something in the background, then use that new point to start a line. But you can't simply compress all these tedious steps by starting a line at the corner of something in the background.5 -
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mahir
Member, Developers Posts: 1,291 ✭✭✭✭✭
I've always seen the benefit of both camps (auto vs manual inferencing). I actually like the OS method the best. It's a nice compromise between the two.5 -
Optionsemmett_weeks
Onshape Employees Posts: 29
For the purposes of stable model regeneration, it's best to avoid projecting model edges into a sketch. The reason is that we don't allow projected edges to change geometry types, so if an edge that projects into a circle becomes tilted with respect to the sketch, the projection will break since it is now projecting as an ellipse. Adding a constraint directly to the model edge is better since it is more likely to continue to work when the model is changed.8
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Optionsbrian_brady
Member, Developers Posts: 505 EDU
I have found that I like projecting key points/vertices from existing geometry onto a new sketch and then "connecting the dots" so to speak. Other than that I use constraints relative to existing geometry (coincident, midpoint, tangent, normal, perpendicular, etc).emmett_weeks said:For the purposes of stable model regeneration, it's best to avoid projecting model edges into a sketch. The reason is that we don't allow projected edges to change geometry types, so if an edge that projects into a circle becomes tilted with respect to the sketch, the projection will break since it is now projecting as an ellipse. Adding a constraint directly to the model edge is better since it is more likely to continue to work when the model is changed.5
Answers
I agree with the title and that makes Onshape pretty awesome piece of software.
I have often cases where new line begins 1mm from something in the back, I hate when cad tries to be smarter than me and snap onto things I don't want.
But we do have shift -function to disable snapping so we could also have button to wake up everything in background?
I'm using Firefox and Safari.
Creo way sounds interesting. I am used to SW where snapping is easy.
I hope people aren't projecting a lot of edges just for trimming in a sketch!!! One thing I like about Onshape, is that it will automatically trim the sketch with the part during the feature creation:
Linked[in]