Toolpath display error.

If you think you've found a bug post it here.

Toolpath display error.

Postby ger21 » Thu Aug 09, 2018 2:34 am

Load this code.

G0 X0 Y0
G1 X10 F500
G3 X12 Y10 I-3 J5
G1 Y11
M30


The arc is shown incorrectly in the toolpath display, although it appears to cut correctly.

Toolpath.JPG
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1143
Joined: Sat Sep 03, 2016 2:17 am

Re: Toolpath display error.

Postby cncdrive » Thu Aug 09, 2018 7:36 am

Gerry, I think (but I will have to study the code a bit longer to make sure) that it displays incorrectly, because the code has an issue and it is not really a valid arc.
It is not a valid or real arc if it has different radius on the 2 sides. In other words when the center point has different distances from the 2 endpoint and so it is not really a center point.
The motion API supports to cut this kind of code too, but the drawing algorithm not.
We have not decided yet if we will want to make the drawing algorithm to handle this type of code or if we want the software to through an error on it and not execute.
There are a few reasons for both and so we could not decide yet.
I will take a closer look at your code later today, because I have some work to do now...
cncdrive
Site Admin
 
Posts: 2263
Joined: Tue Aug 12, 2014 11:17 pm

Re: Toolpath display error.

Postby ger21 » Thu Aug 09, 2018 10:56 am

I didn't even think that the code was bad. Sorry.

Not sure if you should keep it like this, or throw an error?
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1143
Joined: Sat Sep 03, 2016 2:17 am

Re: Toolpath display error.

Postby cncdrive » Thu Aug 09, 2018 11:01 am

Gerry,

Yes, we are also unsure if we want to let this execute or if we want to throw an error,
because on one hand it is a feature that the controller can execute it but on the other hand it is not a real arc, so it is a g-code error.
We will have to make a decision on this...
cncdrive
Site Admin
 
Posts: 2263
Joined: Tue Aug 12, 2014 11:17 pm

Re: Toolpath display error.

Postby ger21 » Thu Aug 09, 2018 12:20 pm

Mach3 has a similar "feature" that you can use to create spirals, by offsetting the end of the arc. I think in Mach3 it's limited to 1/2" or 12mm, and any more any you get an error.
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1143
Joined: Sat Sep 03, 2016 2:17 am

Re: Toolpath display error.

Postby cncdrive » Thu Aug 09, 2018 12:23 pm

I see. We will think about the best solution, probably we will just adjust the toolpath display and will allow this type of errorous code to execute.
cncdrive
Site Admin
 
Posts: 2263
Joined: Tue Aug 12, 2014 11:17 pm

Re: Toolpath display error.

Postby Vmax549 » Sat Aug 11, 2018 4:50 pm

It would be NICE to have

Helical interpolation
Spiral interpolation

For UCCNC.

(;-) TP
Vmax549
 
Posts: 1312
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: Toolpath display error.

Postby cncdrive » Sat Aug 11, 2018 5:07 pm

UCCNC already have both.
Helical interpolation is simply changing the depth axis while there is an arc interpolation on the active plane and ofcourse the UCCNC can already do that on all 3 planes.
Spiral interpolation is also possible as described in this forum thread, just the display is not proper. However spiral interpolation can be done also with real arcs and in this example the arc is not an arc, because the center point is not in the middle and so the radius is not constant, so it is not an arc, but again the UCCNC will interpolate this errorour code too it will just not display it properly.
cncdrive
Site Admin
 
Posts: 2263
Joined: Tue Aug 12, 2014 11:17 pm

Re: Toolpath display error.

Postby ger21 » Sat Aug 11, 2018 5:30 pm

Here's a spiral:

Code: Select all
G0 Z0.1000
G0 X4.0000 Y3.2500 Z0.1000
G1 X4.0000 Y4.1932 Z-0.2000 F50
G2 X4.0000 Y4.1932 Z-0.2000 I0.0000 J-0.1933 F100
G2 X4.0000 Y4.3865 Z-0.2000 I0.00 J-0.1933
G2 X4.0000 Y4.5798 Z-0.2000 I0.00 J-0.3865
G2 X4.0000 Y4.7730 Z-0.2000 I0.00 J-0.5798
G2 X4.0000 Y4.9662 Z-0.2000 I0.00 J-0.7730
G2 X4.0000 Y5.1595 Z-0.2000 I0.00 J-0.9663
G2 X4.0000 Y5.3527 Z-0.2000 I0.00 J-1.1595
G2 X4.0000 Y5.5460 Z-0.2000 I0.00 J-1.3528
G2 X4.0000 Y5.7392 Z-0.2000 I0.00 J-1.5460
G2 X4.0000 Y5.9325 Z-0.2000 I0.00 J-1.7393
G2 X4.0000 Y6.1258 Z-0.2000 I0.00 J-1.9325
G2 X4.0000 Y6.3190 Z-0.2000 I0.00 J-2.1258
G2 X4.0000 Y6.5122 Z-0.2000 I0.00 J-2.3190
G2 X4.0000 Y6.7055 Z-0.2000 I0.00 J-2.5123
G2 X4.0000 Y6.8988 Z-0.2000 I0.00 J-2.7055
G2 X4.0000 Y7.0920 Z-0.2000 I0.00 J-2.8988
G2 X4.0000 Y7.2852 Z-0.2000 I0.00 J-3.0920
G2 X4.0000 Y7.4785 Z-0.2000 I0.00 J-3.2853
G2 X4.0000 Y7.6718 Z-0.2000 I0.00 J-3.4785
G2 X4.0000 Y7.8650 Z-0.2000 I0.00 J-3.6718
G2 X4.0000 Y7.8650 Z-0.2000 I0.00 J-3.8650
G0 Z0.1000
G0 X4.0000 Y7.8750 Z0.1000
G1 X4.0000 Y7.8750 Z0.0000 F50
G2 X4.0000 Y7.8750 Z-0.2000 I0.0000 J-3.8750 F100
G2 X4.0000 Y7.8750 Z-0.2000 I0.0000 J-3.8750
G0 X4.0000 Y7.8750 Z0.1000
M30
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1143
Joined: Sat Sep 03, 2016 2:17 am

Re: Toolpath display error.

Postby Vmax549 » Sat Aug 11, 2018 6:18 pm

I have no idea what I was thinking when I wrote this. What I was working on was tapered thread milling. I currently have to do it with parametric programming a series of lines to approximate teh shape.

What I meant was a Spiraling Helix to cut tapered threads :oops: I have not been able so far to make that work using arcs. BUT it could have been the toolpathing glitch that threw me off base.

I just tried Gerrys spiral and adding a Z stepdown BUT teh Z dro never showed teh stepdown for each layer.

I will work on it more later.

(;-)TP
Vmax549
 
Posts: 1312
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Next

Return to Report a bug

Who is online

Users browsing this forum: No registered users and 1 guest