sketch will not extrude ("The extrude profile is not valid.")

ScottFergTMXEZ · ‎07-06-2023

Attempting to extrude ('Press Pull') from a sketch of an internal (ring) gear which was imported (inserted) as a DXF. Extruding the outer ring fails with "The extrude profile is not valid". Yet Check Sketch: reports "No open loops found in sketch". 'DXF Close Sketch Gaps' also does not help. Nor does 'DXF Bulk Import' with a 'Gap Tolerance' of 0.01 in. Interestingly, I can properly extrude the inner, more complex, portion of the profile. And I can extrude when both the inner and outer (circle) profiles are selected, i.e. the circle is OK. Just the ring between the inner and outer profiles fails. (This is the 'invalid_profile1.f3d attached file.)

The inner profile contains arcs and when I replace them with equivalent cubic Bezier curves in the imported DXF file the extrusion succeeds. Because DXF arcs are represented as start and end angles rather than start and end points, I suspect the calculated start and endpoints for the arcs are not matching up with neighboring segments along the profile at some (excessively?) high tolerance level. Curves are saved with the endpoints and match up OK. (This is the 'valid_profile.f3d attached file.)

I attached a JPG image of the sketch in Fusion for further visual reference.

So what's actually wrong with the profile(s) and how do I fix it? Thanks for any help in resolving this problem!

HughesTooling · ‎07-07-2023

This is really strange! I drew 2 lines across the sketch to see if I could extrude sections of the profile and found will the lines making 4 profiles I can extrude the whole part!

EDIT Please don't attach pictures, just paste into your message. Makes it a lot easier to read and view the picture.

Mark Hughes
Owner, Hughes Tooling
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HughesTooling · ‎07-07-2023

Even stranger, just drawing 1 line from the centre to the outer circle is all that's needed to make it work! @jeff_strater What do you think is going on here?

Mark Hughes
Owner, Hughes Tooling
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g-andresen · ‎07-07-2023

Hi,

The cause is a miserable sketch quality.
I converted them into arcs with a tolerance of 1/1000 mm.

günther

HughesTooling · ‎07-07-2023

Just found that although I got a preview before when I click OK it only creates a cylinder and selects to inner sections! Files attached using 2 extrudes.

But if I use 2 extrudes I can get just the external ring gear.

@g-andresen wrote:

Hi,

The cause is a miserable sketch quality.
I converted them into arcs with a tolerance of 1/1000 mm.

günther

@g-andresen What's wrong with the sketch? The original sketch can create a nice simple (compared to yours) gear.

This is from the original sketch only 2 fillets, 4 splines and an arc for the tooth cutout.

Yours has way more surfaces.

Original sketch also chains and create a nice clean body in Rhino.

Mark Hughes
Owner, Hughes Tooling
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g-andresen · ‎07-07-2023

Hi,

@HughesTooling wrote:

Just found that although I got a preview before when I click OK it only creates a cylinder and selects to inner sections! Files attached using 2 extrudes.

But if I use 2 extrudes I can get just the external ring gear.

@g-andresen wrote:

Hi,

The cause is a miserable sketch quality.
I converted them into arcs with a tolerance of 1/1000 mm.

günther

@g-andresen What's wrong with the sketch? The original sketch can create a nice simple (compared to yours) gear.

1. I know such phenomena as a result of multiple copying.

Yours has way more surfaces.

2. This is due to the selected tolerance when converting.

günther

HughesTooling · ‎07-07-2023

The primary sketch is only made from splines and arcs, Fusion should not have any problem with it.

One side of a tooth is just 3 arcs and 2 degree 3 splines, I wouldn't call that miserable sketch quality.

Can't see any errors in start and end points here, Fusion even detects the closed profiles.

Mark Hughes
Owner, Hughes Tooling
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g-andresen · ‎07-07-2023

Hi,

@HughesTooling wrote:

The primary sketch is only made from splines and arcs, Fusion should not have any problem with it.

One side of a tooth is just 3 arcs and 2 degree 3 splines, I wouldn't call that miserable sketch quality.

Can't see any errors in start and end points here, Fusion even detects the closed profiles.

I just saved the sketch from the given f3d as DXF and showed the result in the screenshots before and after conversion and after reimport into Fusion.

günther

jeff_strater · ‎07-07-2023

@HughesTooling - yeah, that seems like a bug. I created FUS-133735 for it. My offhand guess is that either there is some degenerate curves in there, or maybe the algorithm has some bugs. Thanks for pinging me.

Jeff Strater
Engineering Director

ScottFergTMXEZ · ‎07-07-2023

@jeff_straterThanks for your attention to this! This issue resulted from work on my FMGears add-in, which works essentially by importing a DXF file via the plugin API. I'm fairly certain there are no degenerate curves involved. There are 4 curves and 4 arcs per tooth, a total of 480 segments for the 60-tooth gear. The tooth profile is just repeated around the gear, so examining one shows the structure of the others. Some care is taken to ensure the segments are all connected. (I'd certainly not call it 'miserable'.) It has been problematic that the DXF Arc format does NOT specify the endpoints, so an importer calculating them from the start and end angles and other parameters and getting matching endpoints is dependent upon the precision presented and the calculations themselves. Prone to error. Perhaps the DXF import API has a gap tolerance I can tweak. But as best as I can tell in Fusion, they're all connected properly in this sketch anyway. DXF Curves do not have that problem, so I might just represent all the segments as curves, eliminating arcs, to avoid problems moving forward.

For completeness, I've attached the actual DXF file used to generate the Fusion sketch.

BTW, where can I track the FUS-133735 report you've created for this?

Thanks!

Scott

HughesTooling · ‎07-08-2023

@ScottFergTMXEZ Could you make your add-in work like Fusion's spur gear add-in where you only create a sketch for one tooth. Then use that as an extrude cut and pattern the extrude cut? Something like the attached file?

Mark

Mark Hughes
Owner, Hughes Tooling
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ScottFergTMXEZ · ‎07-08-2023

@HughesTooling wrote:
Could you make your add-in work like Fusion's spur gear add-in where you only create a sketch for one tooth. Then use that as an extrude cut and pattern the extrude cut?

The short answer is, "Of course!" The long answer is, "No way!" My (C#) computational library that does all the work has a history of over 26 years of development and is shared with my free (Windows) program 'GearDXF'. The library builds the gear and exports a DXF which is import and extruded by the add-in. Honestly a bit of a hack, but allows one code base to support both programs and has worked fine, at least up until I discovered this problem.

ScottFergTMXEZ · ‎07-11-2023

@jeff.strater An interesting observation for this (potential) bug is that if I load the DXF file using the "Upload" button in the Project window it creates a file with a sketch that succeeds when extruding the ring. Whereas using the "DXF Insert" or "DXF Bulk Import" menu commands fail. So different loading methods get different results!