topic Re: Can't move point in sketch in Fusion Support Forum

Can't move point in sketch

williamw003 — Tue, 16 Sep 2025 09:38:17 GMT

i'm following a video tutorial where the right point is symmetrically constrained with the left. However, in the future he clicks on the left point and drags it and the right one follows, but for some unknown reason mine does not work and keeps making this useless purple circle. There is no coincident constraint on the points or anything except for symmetry constraint, but the guy in the video has it too and it works fine. Anyone know why? Thanks

(view in My Videos)

Re: Can't move point in sketch

John_Wright — Tue, 16 Sep 2025 10:18:03 GMT

The purple circle is a piece of projected geometry.

Try turning off the tick box that says "Projected Geometry" and see if you can grab the point you want.

Do you have a link to the tutorial? It may be that unideal techniques are being used here.

Re: Can't move point in sketch

williamw003 — Tue, 16 Sep 2025 10:27:30 GMT

i've tried ticking projected geometry off, and i still can't grab it. The point will still revolve around a circle if i drag. The link is:

https://www.youtube.com/watch?v=o5rcAv7xVUo

7:04

Re: Can't move point in sketch

John_Wright — Tue, 16 Sep 2025 10:49:13 GMT

There are 2 coincidenal points here. One on the end of the line you want, and one that joins the projected arch to the pojected line. You need to delete the correct one, and click on the correct one.

If it was me modelling this, I certainly wouldn't have projected the entire face as there is load of geometry that isn't required. And, I wouldn't model it "wrong" to then correct it, You can get all the geometry you need from projecting two points.

Also, I have no idea why people don't use part of the origin as there middle point on parts that are going to be symmetrical....You can model most of this part in one half and then mirror it....

Re: Can't move point in sketch

williamw003 — Tue, 16 Sep 2025 12:15:58 GMT

hm, the coincidents wouldn't pop up either when i hovered/clicked on the point until after a bunch of finickiness. Strange. Works now, thanks

Re: Can't move point in sketch

davebYYPCU — Tue, 16 Sep 2025 12:27:06 GMT

Why???

would you connect that line to the corner, when it should be 10mm away from it.

same for the semi circle, if you watch to the end, you can cut a lot of steps, by just doing the finished stuff..

Might help….

Re: Can't move point in sketch

TheCADWhisperer — Tue, 16 Sep 2025 20:20:14 GMT

@williamw003

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Attached is an alternative technique.

Re: Can't move point in sketch

John_Wright — Wed, 17 Sep 2025 07:55:57 GMT

100% agree. Thats exactly how I would tackle this.

There seems to be a strange teaching method doing the rounds where you're shown what not to do (but it looks like an important step), then told why its wrong, then how to correct it. I find this odd.

Imagine a driving lesson in this manor: Drive straight on towards that lamp post, you hit a lamp post, now im going to show you where you went wrong...

At University (albieit a very long time ago) I was shown "best practice", then the potential pitfalls where highlighted.

Re: Can't move point in sketch

williamw003 — Wed, 17 Sep 2025 10:05:46 GMT

(view in My Videos)

i'm also having trouble with following the rest of the video. I'd first followed him step by step, r-patterning it across and manually applying filet to them all. It worked, but this one bar in the middle kept having an issue where the bottom was distorted, so i deleted them all, redrew the rectangle and tried applying filet to one bar with the intention of r-patterning it across. Now it keeps giving an error no matter what i do

Re: Can't move point in sketch

davebYYPCU — Wed, 17 Sep 2025 11:16:53 GMT

Ah, even though the tutorial is not great, you have some rookie mistakes too.

The fillets work if done as 2 steps, do the 2 vertical edges first to make the rounding. (1mm). (Not sure why he did not have the 2 point circle both ends - it works both ways.)

After that Select the top face (as second fillet command) will fillet at 1mm. In the video that only just turned up, you did not select the edges at the top end, might make a difference.

To stop the pattern failing, start the pattern, change the type to Features,

from the timeline, select the Emboss and 2 fillet icons off the timeline. Set the pattern values, works for me.

Blue and white Sketch article should keep you awake at night. (All sketch articles should be black or purple.)

You have a few duplicate flange bodies, 2, 3 and 4. Can be deleted.

I'll presume the Whisperer has done his normal best quality, so not going to provide a "my way" version.

Might help...

Re: Can't move point in sketch

TheCADWhisperer — Wed, 17 Sep 2025 18:55:33 GMT

@williamw003 wrote:

i'm also having trouble with following the rest of the video.

@williamw003

Check back later - I am recording a video on alternate instruction technique.

Re: Can't move point in sketch

TheCADWhisperer — Thu, 18 Sep 2025 01:51:04 GMT

@williamw003

Here is an Alternative Instruction technique for the geometry.

https://youtu.be/ZhG7WNBelGk

Re: Can't move point in sketch

williamw003 — Thu, 18 Sep 2025 06:27:24 GMT

thanks