Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Unable to select bottom contour in 2D Contour

7 REPLIES 7
SOLVED
Reply
Message 1 of 8
etfrench
196 Views, 7 Replies

Unable to select bottom contour in 2D Contour

Clicking on the bottom contour of this timing belt pulley results in the vertical face being selected.  Selecting multiple of these show just the bottom contours selected, but no toolpath is generated.

etfrench_0-1697753497352.png

Clicking on the bottom face will create a toolpath, however it cuts on both sides of the face which is not the desired outcome.

 

If the face is projected to a sketch, the toolpath can be created.  This should not be necessary.

ETFrench

EESignature

7 REPLIES 7
Message 2 of 8
jscott6SWZG
in reply to: etfrench

That’s what I think but it’s usually quicker to make a tool path sketch if it doesn’t work after three tries

Message 3 of 8
matty.fuller
in reply to: etfrench

Works perfectly fine for me, one click for a valid contour...

 

mattyfuller_0-1697777999391.png

 

mattyfuller_1-1697778030356.png

 

Your file had 5 tiny chains selected, and as you can see they are all Closed Chains which means they probably overlap themselves, which is why no toolpath calculated.

 

mattyfuller_2-1697778104830.png

 

I suspect this is a user issue, not software.

 

Message 4 of 8
etfrench
in reply to: matty.fuller

One click is not working for me.  Each click is selecting the vertical face.  That toolpath shows what happens when the bottom contour was selected on several adjoining arcs. Attached video shows the bug.

 

All of the arcs in each tooth were trimmed at each end to the next arc.  There are 90 teeth, so there is a 4 degree angle in each tooth.  There are no overlaps in the tooth form or the circular pattern.  Fusion 360 appears to only be accurate to 6 decimal places.  Here is the output for the endpoints of two left hand arcs in the tooth form from my 2D CAD program:

 

#1 [Arc], UID: 5, Layer: 0, Color: 15:(LP), LnType: 0:(LP), Width: 0:(LP), #Pts: 3
p1: 0.01274864",1.67737270"
p2: 0.00637435",1.67740256"
p3: 0.00000000",1.67740819"
Center Pt: 0.00170350",-0.00001208", Radius: 1.67742114", Length: 0.01274872"

#2 [Arc], UID: 11, Layer: 0, Color: 15:(LP), LnType: 0:(LP), Width: 0:(LP), #Pts: 3
p1: 0.02268324",1.66839435"
p2: 0.01942696",1.67477677"
p3: 0.01274864",1.67737267"
Center Pt: 0.01268240",1.66731386", Radius: 0.01005903", Length: 0.01465188"

ETFrench

EESignature

Message 5 of 8
HughesTooling
in reply to: etfrench

@etfrench Have you got the New Chaining preview enabled?

 

It seems to work with one click if I zoom in for the selection but there seems to be some odd leads.

Clipboard01.png

Odd leads also visible in @matty.fuller picture.

Clipboard02.png

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 6 of 8
HughesTooling
in reply to: etfrench

@etfrench I noticed in your sketch one of the arcs is not constrained. If I add a concentric constraint it makes the arc constrained but then the profile becomes open somewhere! 

Clipboard01.png

What I found helps is to delete the unconstrained arc and extend the other.

Clipboard02.png

 

Now when I select the bottom edge in the manufacture workspace I get a good toolpath without the extra leads. Also note the outer cylindrical surfaces are now merging so points towards a small error in the original sketch.

Clipboard03.png

 

 

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 7 of 8
HughesTooling
in reply to: etfrench

Looking at the sketch a bit more and it's a lot more complicated than it needs to be and seems like there are some inaccuracies. The 4° angle shows a small error, how did you create this line? If I type 4° in it makes it correct. Did you just sketch or rotate manually then add the angel without actually typing the number? You also have a 0.034 dimension one side and 0.033 the other. Dimensioning seems pretty chaotic.

HughesTooling_0-1697820053062.png

 

If you add the small fillets to the model rather than the sketch you can simplify the sketch to something like this. Also take advantage of construction lines to create symmetry. See attached file. Sizes might not be quite right but I did my best to get the sizes off your sketch, note sketch is now fully constrained.

Clipboard01.png

 

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 8 of 8
etfrench
in reply to: HughesTooling

Adding the concentric constraint and splitting the contour in half, then mirroring it has fixed it.  The concentric constraint also changed the endpoints of the two left hand arcs so they are now identical.  Both endpoints changed to p1: 0.01275891",1.67737260".

ETFrench

EESignature

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report