Cutter Radius Compensation ( G40 , G41 , G42 )

Here is where you can request new features or special features.

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby cncdrive » Tue Dec 19, 2017 2:40 pm

Hi Brendon.
I got the dxf file and generated a toolpath from it and set the G42 to tool dia=1 and got the results on the attached printscreen.
I'm not sure where the issue was in mach3 or if the result on the picture is what you expect to happen? Please check the picture...
Attachments
G42D1.png
cncdrive
Site Admin
 
Posts: 2457
Joined: Tue Aug 12, 2014 11:17 pm

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby A_Camera » Wed Dec 20, 2017 8:48 am

cncdrive wrote:Hi Brendon.
I got the dxf file and generated a toolpath from it and set the G42 to tool dia=1 and got the results on the attached printscreen.
I'm not sure where the issue was in mach3 or if the result on the picture is what you expect to happen? Please check the picture...

Hi Balázs,

Does this mean we can expect a Christmas present from you...? ;)

I'd love to be able to start using G40/G41/G42 again.
A_Camera
 
Posts: 476
Joined: Tue Sep 20, 2016 11:37 am

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby Battwell » Wed Dec 20, 2017 11:35 pm

Set tool diameter to 12 not 1
The issue is if the tool radius is larger than a segment- it should roll around but in Mach 3 it gouges where pointed to
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 415
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby Battwell » Fri Dec 22, 2017 12:43 pm

to be fair- since using vectric products to post code for my machines- where it is so quick to recalculate and re post/run code i rarely use g41/42 now.
i used to use it all the time when running my parts with parametric code- but havnt done that for a couple of years now either.
there are a huge amount of things that can upset it working correctly. - with my old biesse machines it worked perfectly until you had more than 2 calculations on a line- then it would stumble!
i think when you beta release it- its going to require some serious testing pre releasing to the untrained public
how many people actually use it these days-?- in the real world. (hobby world) id guess most wouldnt have a clue how to implement it with lead ins/outs etc.
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 415
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby ger21 » Fri Dec 22, 2017 2:20 pm

how many people actually use it these days-?- in the real world.


I do. It's pretty common with the big Italian machines. I've been using it for 20 years, on a Masterwood, and now a Morbidelli. And I also use it for most parts that I run in Mach3 on my old machine.
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1259
Joined: Sat Sep 03, 2016 2:17 am

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby Derek » Fri Dec 22, 2017 6:05 pm

I would like to learn it so that I can compensate for cutting errors at the machine. I've never used it though so there is that. Some times trying to dial in that last thousandths via CAM can be arduous.
Derek
 
Posts: 299
Joined: Mon Sep 05, 2016 9:57 am

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby cncdrive » Fri Dec 22, 2017 10:40 pm

I have also never used G41/G42 myself, but now that we implemented it into the UCCNC I fully understand it's working and also it's limitations.
Because it is clearly defined how it has to work mathematically and we wrote the algorithms I see are limitations. The limitations comes from that the codes are based on one movement look ahead and therefor there can be cases especially on path with lots of short and different direction movements and especially with large offsets compared to the movements dimensions then the offsets will be not perfect.
It is then not perfect because of how it has to work.

CAM softwares calculating the offset with totally different mathematical algorithms which algorithms looking at the path as one big piece and doing the calculation on all the path instead of just looking one movement ahead and going along the path.
Ofcourse such algorithms can't work on a CNC controller like how the G41/G42 can, because while the G41/42 needs only a small amount of time to calculate that one movement at a time, the algorithm in a CAM software may require a serious amount of time to complete, because it looks the whole path and so the calculation is time costy and so it can't work in "realtime" is why the simple and fast G41/G42 still remained the standard on CNC controllers eventhough it has lots of limitations because how it works, how it has to work.
So, I'm also prefering regenerating the path with the CAM over the G41/G42 in most cases, what I think the G41/G42 is perfect for simple paths and/or small offsets for example tool wear size offsets.

Maybe in the future when computers will have a so high computing power that advanced ray tracking algorithms which are implemented in CAM softwares for offset calculations can be computed in a short enough time then the G41/G42 will be replaced with these codes, but I also think that it will probably take a few decades if it will ever happen.
cncdrive
Site Admin
 
Posts: 2457
Joined: Tue Aug 12, 2014 11:17 pm

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby Battwell » Sat Dec 23, 2017 11:35 am

As ger mentions - it is widely used on the Italian machines. These are mainly point to point machines with very limited cv . ( from what I've seen running the Biesse etc). Maybe that's why they handle it quite well.
I ran the Italian way for around 4 years before converting the controls .
My old Biesse wouldn't import anything so every line was typed into the control . But!:::

The problem is going to arise when someone imports from cam- for example a simple square.
They cut the square
Then they measure it and find it's off by 0.1mm offset.
So they re run the path with that 0.1mm offset removed from the tool diameter.(g41/42)
Then they find they have a rhombus instead of a square- because the g42 has used the first and last sides as the lead in/ lead out. - so now they have a scrap part
Instead to use it they have to either
A. Add a lead In / out line in the code manually before running ( most wouldn't have a clue)
Or go back into cam and recalculate- post and run
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 415
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby ger21 » Sat Dec 23, 2017 11:42 am

This really shouldn't be an issue. If people have never used G41/G42, they aren't likely to start using it.
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1259
Joined: Sat Sep 03, 2016 2:17 am

Re: Cutter Radius Compensation ( G40 , G41 , G42 )

Postby Battwell » Sat Dec 23, 2017 12:45 pm

ive just downloaded the christmas present - thanks balacz!
il give it a whirl- when im sober enough to do it properly!
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 415
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

PreviousNext

Return to Feature Request

Who is online

Users browsing this forum: No registered users and 1 guest