A cad software is only as good as the basic sketching is

tore_thoresen

...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. 

3dcad

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.

lougallo

If the face is shared with the sketch plane we do inference those entities.  What browser are you using?

chris_8

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.   

3dcad

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?

brian_brady

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.   

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.

mahir

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. 

emmett_weeks

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.

brian_brady

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.

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).

3dcad

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.

lougallo

If the face is shared with the sketch plane we do inference those entities.  What browser are you using?

chris_8

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.   

3dcad

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?

brian_brady

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.   

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.

tore_thoresen

Thanks, I'll try 'use/project'. 
I'm using Firefox and Safari. 
Creo way sounds interesting. I am used to SW where snapping is easy. 

mahir

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. 

emmett_weeks

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.

brian_brady

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.

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).

tore_thoresen

Thanks for all folks, I just started to like the OS way, put thanks to the Free Plan change, I will probably never get back to OS after 15th of Des.

fastwayjim

brian_brady said:

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.

Couldn't agree more, the workflow for creating constraints in Creo is both great and terrible at the same exact time.

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:

3dcad

in addition to @fastwayjim 's tip, if that feature makes things difficult for you (ie. need to select 100 areas to get full extrude for your sketch) then you can select whole sketch from feature list.