How to trim/extend projected curves in sketcher?

[phbalance]

I am creating a part which needs to reference off of imported data in order to match existing surfaces. When I go into sketch mode, I use the project button to "copy" the edges from the imported surface. The section is basically a "U" shape - 2 vertical lines, a horizontal arc, and corner rounds. I do not want the rounds however. How do I trim/extend the section so I get sharp corners?

 

[Dave K]

Rather than using project, and trim/extening the lines, how about creating 3 new lines in the sketcher, and constraining those 3 to be colinear with the reference lines, coincident at the top of the U, forming a squared off U.



-Dave
Everything should be designed as simple as possible, but not simpler.

 

[phbalance]

Actually, it's a bit more complicated than that. The horizontal arc I mentioned is not a simple arc. It is a spline, so it would not be accurate if I didn't "copy" it. Is there no simple way to make the 2 end points meet? Any other suggestions?

 

[feadude]

in sketcher delete rounds, zoom out to where both lines of a corner fall within the selection ball radius then goto edit, edit curve and select trim corner.
This option trims two curves to their intersection point, thereby forming a corner. The corner that is created depends on the objects selected. As with all Edit options, the portion of the curves selected, with respect to their intersection point, is trimmed/extended. When you select curves for a corner trim, position the selection ball so that it includes both curves.
If the selection ball contains only one curve, an error message is displayed:

No Valid Curves

 

[phbalance]

AARGH!!

feadude: I tried your suggestion too, but it's giving a "cannot corner trim this curve in sketcher" error. I can trim all I want if the sketch features cross each other, but if the sketch features have a gap between them, the corner trim doesn't work. The trim corner option doesn't seem to work for projected curves and splines, but it works with arcs and lines. I am getting around it by "tracing" the imported edge with arcs. Not happy about it, but it's close.

We do this all the time with Pro/E and Solidworks parts. I can't believe UG is not capable of doing such a simple operation.

 

[cowski]

Is this feature going to be parametric? (if the imported shape changes, your sketch automatically updates?)

If the answer is "no", you can skip the sketcher entirely.

Even if the answer is "yes" you can probably skip the sketcher entirely.

 

[feadude]

If associativity is not an issue:
when you project curves in sketch turn the "Associative" ( it looks like two chain links) off and then project curves then delete the rounds and trim/extend corners. It works . I just tried it.

 

[phbalance]

Okay, thanks guys for the suggestions. I found another way to do it. In sketcher, edit curve -> arc length -> and change the length of the projected curve until it crosses the other sketch curves. Then quick trim to form the sharp corner.

The feature does need to be parametric.

Skipping the sketcher entirely? As a seasoned Pro/E user, we use sketches to form most of our curves. It's tough to grasp the concept of these "floating" curves. Guess I need more practice to get used to it. I've only been using UG for about a week now.

 

[ewh]

Seeing as how you are new to UG, I would suggest doing it however is the easiest for you, which means use the sketcher. Just be aware of the potential power you now have when it comes to approaching problems from different directions.

 

[feadude]

I am not able to change the length of the curve using "arc length" without moving the rest of the geometry and loosing the original shape?

 

[phbalance]

That's weird. It works fine for me. I have the associativity turned on. The curve stays true after arc length operation.

 

[ewh]

feadude, do you have something constrained to the end of the curve?

 

[feadude]

no I do not. I do not really understand how changing the length of the arc will help the trim operations.

 

[ewh]

Seems to be a bug where the trim corner command won't extend certain curves. If you lengthen the curve beyond the intersection point, you can then trim the corner.

 

[Azrael]

Can´t you skip the sketch and extract the curves in space and trim the extracted curves?

 

[mjcole]

Just sketch a temporary line that you can use to extend the curves you want to trim. then use the trim curve option the icon with the eraser to trim the curves on the other side.

Then you can delete the temporary line after it's served its purpose.

Michael

 

[HellBent]

Yeah ewh...I get that a lot. Some curves just won't automatically extend to the trim object. You often times have to extend the curve beyond the trim object and then trim it back. A note for the noobs....when you're trimming curves in 3d try to get in the habit of selecting the "shortest 3d distance" trim method rather than by WCS...WCS relative trims can really mess you up...lol.