CAD Forum

Every dang time I give in and use Offset Sketch Entity I regret it!
Argh.

Make just a few simple upstream changes and every offset relation gets trashed and I have to re-do the sketch relations manually.

You'd think I'd learn my lesson by now but no...

I'm cautious with offsets. If it's only a couple entities, I do it the hard way. If I'm ever forced to sketch a full sheet metal section, I don't use offsets. To much risk of disruption if entities need to be added or subtracted from the offset chain.

So much agreement!

I use it fairly often. I do have relations blow up occasionally, but when it does it's generally not too difficult to fix, so it's not enough to make me stop using it.

When sketch offsets blow up with edits, it's usually stuff other than lines. So arcs, splines, other curves. Under most circumstances, a straight line will usually project and offset as a straight line. Not so for any other type of curve. If you section a cone normal to the axis you get a circle. If you tilt the plane you get an ellipse, a parabola, hyperbola.

So if you stick to things that project and offset as lines, and just manually sketch/dimension the rest, you will be better off.

I just wish it were easier to use. Why isn't there a "follow tangent" option? Why can't I select using a window? I have to select each line segment individually, and hope I don't accidentally click on something that causes it to screw up.

SPerman wrote: ↑Thu Sep 16, 2021 3:41 pm I just wish it were easier to use. Why isn't there a "follow tangent" option? Why can't I select using a window? I have to select each line segment individually, and hope I don't accidentally click on something that causes it to screw up.

I just select the things I want, and then extend/trim or connect with sketch fillets.

Another alternative is to select a face to offset rather than edges, SW automatically gets the outside loop. You can force it to automatically get an inside loop by picking the face and ctrl-selecting one edge of the inside loop. Then changes won't be as disruptive.

Thanks for that tip. I will have to give it a try next time I use offset.

SPerman wrote: ↑Thu Sep 16, 2021 3:41 pm I just wish it were easier to use. Why isn't there a "follow tangent" option? Why can't I select using a window? I have to select each line segment individually, and hope I don't accidentally click on something that causes it to screw up.

There is a 'Select Tangency' in the right click menu

SPerman wrote: ↑Thu Sep 16, 2021 3:41 pm I just wish it were easier to use. Why isn't there a "follow tangent" option? Why can't I select using a window? I have to select each line segment individually, and hope I don't accidentally click on something that causes it to screw up.

Please watch the gif below and tell me what I am doing wrong. (2020 SP5)

SPerman wrote: ↑Fri Sep 17, 2021 8:55 am Please watch the gif below and tell me what I am doing wrong. (2020 SP5)

Offset.gif

When I use Offset Entities it's almost always on other sketch entities. I just tried on edges of a model similar to the one you posted, and got the same results you did. Sorry about that.

@SPerman The Select Chain option seems to be for Sketch Entities, not Raw edges.

Start the sketch, do not start the Offset command.
Right click the same edge as you did in the gif
"Select Loop"
Click the yellow arrow to select the proper loop, if necessary
Start the Offset Entities command
Now it should work as expected.

Hope this helps,

Ray

Thanks for that. I will give it a try.

Face selection is key stability. SolidWorks is somewhat "smart" about that face selection, you can add features before the sketch offset and even suppress and the sketch offset will update accordingly. Unfortunately you can't really seem to 'edit' that initial face selection, the Display Relations makes it appear to be an edge selection.

Maybe a dumb question:
You cannot 're-link' broken offset entities/converted entities, can you?

I think that's the biggest curse...

berg_lauritz wrote: ↑Mon Sep 20, 2021 8:14 am Maybe a dumb question:
You cannot 're-link' broken offset entities/converted entities, can you?

I think that's the biggest curse...

No, I don't believe that you can. Which is a major downfall of this practice (IMO)

berg_lauritz wrote: ↑Mon Sep 20, 2021 8:14 am Maybe a dumb question:
You cannot 're-link' broken offset entities/converted entities, can you?

I think that's the biggest curse...

That is exactly the trap I set for myself every time i use Sketch Offset. As noted by others in this thread, there ARE a lot of strengths to the SO command, and a lot of flexibility. Its just the little problem of what to do if you need to go back and change the referenced geometry. Sometimes its not so bad, just delete the Offset relation and offset manually.

Normally I just offset manually from the start, using lots of construction lines at corners with equal relation (I usually am dealing with just straight lines). But sometimes I just need to do it quickly.

dpihlaja wrote: ↑Mon Sep 20, 2021 8:22 am No, I don't believe that you can. Which is a major downfall of this practice (IMO)

I don't think it warrants not using it. Worst case you have two options:

1. Delete and recreate the offset. (Can cause problems downstream but not always bad)
2. Delete broken relations and recreate dimensions and relations to mimic the intent to maintain downstream integrity.

Option 2 is what you guys are advocating to begin with, so why not start with an offset and let it work for as long as possible knowing you can fall back to it?

Again, the face select will provide maximum stability since faces rarely go away. This is a really old function that sorely needs some attention, like the ability to repair/edit the face selections.