G41/G42 discussion.

Post anything you want to discuss with others about the software.

Re: G41/G42 discussion.

Postby ger21 » Thu Jan 25, 2018 11:11 pm

Battwell wrote:again... how many people actually use this feature now.? i mean - in reality ???


I use it for everything, even in Mach3, except for the few times it doesn't work.
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1116
Joined: Sat Sep 03, 2016 2:17 am

Re: G41/G42 discussion.

Postby cncdrive » Thu Jan 25, 2018 11:38 pm

I've checked this code too now and I see why it fails to make a good offset path.
It is a bit late night here now, but I can explain it tomorrow if anybody interested in the details.
This example is again unfortunately a case when the algorithm just can't work properly.
The code also fails in Mach3 and it should fail in any softwares in my opinion, because the reason for the failure of this code is the weakness of the G41/42 offset calculation algorithm which is that the algorithm is going through the path looking one ahead and finding connection points of the offset lines and perpendinculars.
cncdrive
Site Admin
 
Posts: 2187
Joined: Tue Aug 12, 2014 11:17 pm

Re: G41/G42 discussion.

Postby Vmax549 » Thu Jan 25, 2018 11:51 pm

I did some digging in teh latest Haas NGC control. It does 1 block lookahead PLUS checks the next 3 blocks ahead to check for interference. You can set it up for Fanuc or Yasnac mode. This can prevent teh gouging in tight corners. It appears that one version will simply error out but teh other can rewrite teh contour code to NOT gouge but will change the contour slightly.

Just a thought, (;-) TP
Vmax549
 
Posts: 1190
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby cncdrive » Thu Jan 25, 2018 11:53 pm

Terry, the problem is not tight corners.
cncdrive
Site Admin
 
Posts: 2187
Joined: Tue Aug 12, 2014 11:17 pm

Re: G41/G42 discussion.

Postby Vmax549 » Fri Jan 26, 2018 12:05 am

I was referring to teh example code where you have a corner then a very short segment before another corner. That is where a segment between corners that is less than teh tool radius and where just teh rotation of teh tool around teh endpoint(outside corner radius) gouges the contour. That is where teh Haas 1+3 helps to prevent gouging. Before it makes motion to do a corner radius it checks ahead 3 blocks to see IF it will hit anything.

Just looking at HURCO and it is adjustable between1-8 lookahead for Comp.

Just a thought, (;-) TP

(;-) TP
Vmax549
 
Posts: 1190
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby ger21 » Fri Jan 26, 2018 1:04 am

Perhaps there are better algorithms out there?
https://www.sciencedirect.com/science/a ... 851730009X
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 1116
Joined: Sat Sep 03, 2016 2:17 am

Re: G41/G42 discussion.

Postby cncdrive » Fri Jan 26, 2018 7:16 am

Well, they write "Since the algorithm uses the exact part geometry", which suggests that it requires the part geometry to be known and so it is like a ray tracking algorithm.
G41/42 does not know the part geometry in advance is the problem... the paper description talks about using the algorithm in CAM softwares which is fine, there are much more advanced algorithms ofcourse when the algorithm knows the whole path and when there is enough time available etc. And finally this type of algorithms requires a closed path to be offset or if the path is not offset then the algorithm can only walk around the opened path offsetting it on both sides (around). If you check the figures on the linked site you can see approximately how it works, it works the way like a ray tracking algorithm and not like a G41/42. Again, there is a huge difference in what datas are available and what are the requirements for the algorithm to work and what are the results.
I know what I'm talking about, because you know we also made a basic CAM module for the UCCNC which uses ray tracking algorithm, but that could not work as a G41/42, because as said the requirements for an algoritm like that is different than what is available for a task of G41/42 and also the result is different, because it can only fully offset a path around and not running along the path with an offset.
I know it is not easy to see and understand the differences without actually implementing both these algorithms or at least studying these deep enough and it is also hard for me to properly describe these things in English, but beleive me that I know what I'm talking about, because I already implemented both algorithm types. :)
cncdrive
Site Admin
 
Posts: 2187
Joined: Tue Aug 12, 2014 11:17 pm

Re: G41/G42 discussion.

Postby Vmax549 » Fri Jan 26, 2018 7:43 am

THEN there is the old DIY tool comp uncut vector syndrome :D

Can you fix this in UCCNC ??
Attachments
UncutTC.jpg
Vmax549
 
Posts: 1190
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby cncdrive » Fri Jan 26, 2018 7:55 am

It will be hard without having the code and seeing the problem.
cncdrive
Site Admin
 
Posts: 2187
Joined: Tue Aug 12, 2014 11:17 pm

Re: G41/G42 discussion.

Postby Battwell » Fri Jan 26, 2018 11:06 am

the sample i showed above is the same profile i cut using the biesse. originally all my coding was parametric so even angles were specified as trigonometry. so the control didnt know what it was going to cut until it got to that line and calculated the trig etc. (point to point controller- no cv on it)
but it did offset that part properly (part was a lot more complex - just a snippet that fails was shown)
so - basically- the italians had worked out how to do it in the early 90s.
if i broke say a 12mm cutter i could just select another- eg 14mm from my tool table and re run the program fine.
referring to my sample pic above:
when it came to the lower segment (where you see it tapering in as a gouge- the original control would follow the line then create a smooth radius out to avoid the inside corner.( smaller segment than tool radius) rounding the next corner (creating the 90deg sharp corner) and carrying on the straight section as normal
this makes me think they must have been using the circumference as the reference - not the centre point- if that makes sence
Uc300eth on router and mill
If they say it can't be done- I find a way!
Battwell
 
Posts: 351
Joined: Sun Sep 25, 2016 7:39 pm
Location: South Wales. Uk

PreviousNext

Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 2 guests