CAD Forum

Took me a while to realize that I must manually create a plane at end of the curve, it's not part of the sketch feature definition. I did see that if the curve is selected when new sketch command is started it will create a plane for me, but which end of the curve seems to be up to SW.

Anyway, now I'm in a sketch that's normal to a curve at a point but how can I constrain a sketch element to the inherent pierce point? Majority of the time that I'm sketching on a plane that's defined as normal to a curve at a point the only logical reference point is the pierce point. I could explain how to do this in SE off the top of my head without even seeing it. Incase my question is poorly explained I demonstrate what I'm thinking using SE with a quick random shape.

OK, if you are trying to sweep a round shape along a curve, then solidworks has an easy step.

Just select the curve, and select circular profile. However, if you just used something round as an example, and your real shape will be more complex, then you can use planes.
Alternatively, if you wanted the sketch plane somewhere along the curve, you will have to create some sort of point there to place the plane on. Either a reference point or a point from another sketch.
Then, after sketching on the plane Is this what you want?

dpihlaja wrote: ↑Thu Jan 20, 2022 8:17 am OK, if you are trying to sweep a round shape along a curve, then solidworks has an easy step.

Just select the curve, and select circular profile.
image.png

However, if you just used something round as an example, and your real shape will be more complex, then you can use planes.

image.png

Alternatively, if you wanted the sketch plane somewhere along the curve, you will have to create some sort of point there to place the plane on. Either a reference point or a point from another sketch.
Then, after sketching on the plane
image.png

Is this what you want?

Profile shape was just example, I should have used a square. I got the plane added. Problem is; in your last screen shot I do not get "make pierce" option, only Anchor. That is what I'm trying to find.

bnemec wrote: ↑Thu Jan 20, 2022 10:49 am Profile shape was just example, I should have used a square. I got the plane added. Problem is; in your last screen shot I do not get "make pierce" option, only Anchor. That is what I'm trying to find.

normalToCurve_SW.gif

Select the actual curve entity instead of trying to pick the end. Not at all intuitive, but it works.

bnemec wrote: ↑Thu Jan 20, 2022 10:49 am Profile shape was just example, I should have used a square. I got the plane added. Problem is; in your last screen shot I do not get "make pierce" option, only Anchor. That is what I'm trying to find.

normalToCurve_SW.gif

Yes, as mike points out, you need to select the curve instead of the point. Not sure why you can't make it coincident with the end point, but....

Make pierce is specifically for curves and lines that intersect a plane.

mike miller wrote: ↑Thu Jan 20, 2022 11:07 am Select the actual curve entity instead of trying to pick the end. Not at all intuitive, but it works.

dpihlaja wrote: ↑Thu Jan 20, 2022 11:14 am Yes, as mike points out, you need to select the curve instead of the point. Not sure why you can't make it coincident with the end point, but....

Make pierce is specifically for curves and lines that intersect a plane.

Thank you. So do you both punch my idiot card or just the first to respond?

I miss SE...

bnemec wrote: ↑Thu Jan 20, 2022 12:00 pm Thank you. So do you both punch my idiot card or just the first to respond?

I miss SE...

LOL. No....we've all been through that!

After editing the curve table a few times:
I don't know...

bnemec wrote: ↑Fri Jan 21, 2022 5:05 pm After editing the curve table a few times:

image.png

I don't know...

It would self-intersect at that diameter. Meanwhile SWX just pukes out some geometry and it's up to you to notice what's wrong.

SE won't let you do it; the error message is what alerted me to the problem on the SWX side.

mike miller wrote: ↑Fri Jan 21, 2022 5:47 pm It would self-intersect at that diameter. Meanwhile SWX just pukes out some geometry and it's up to you to notice what's wrong.

SE won't let you do it; the error message is what alerted me to the problem on the SWX side.

I see it now, thank you. My bad. I don't see any warning or error message in SW. I'm assuming you tried copying my helix table into SE and that's where you got the error message? We have SE 2019, looks like you're newer.

After fixing the self-intersect everything better. I should have known to look for that. I guess I was spoiled to SE error. I'm on fence about letting the software try to solve, but would like if it informed me of my error.