G41/G42 discussion.

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

G41/G42 discussion.

Postby ger21 » Tue Dec 26, 2017 3:08 pm

I've played around a bit with the new G41/G42, and have some comments/suggestions.

1) Your implementation of how comp is applied seems to me to be a bit non-standard. Imo, comp should be applied during a lead-in move. As it is now, comp appears to be using the previous tool location to determine how to apply the comp. This seems to cause unnecessary errors.
I can run code that works fine, but sometimes throws an error, depending on where the tool happens to be. This requires additional moves to be added prior to the lead-in move, to avoid these errors. In some cases, depending on tool position, UCCNC does apply the comp like I am expecting. But most of the time, it does not.

If you apply the comp during the lead-in move, then as long as the lead in move is correct, you eliminate the first three of your five warning messages. As long as you specify that the user needs a lead-in move longer than the tool radius, most of your problems go away.
This is how LinuxCNC does it. http://linuxcnc.org/docs/2.6/html/gcode ... mpensation
And how the controls I've used on high end Italian routers as well.
It's fine, imo, if you don't allow arcs for lead-in moves.

2) Comping an outside corner should always result in the tool "rolling around" the corner. This is how basically all CAM programmed g-code is written. I use G41/G42 to cut cabinet parts, which are nearly always rectangular, with square corners. I don't want the tool to stop at each corner, when it can roll around the corner at higher speeds.
I can't think of any situation where it wouldn't be desirable to roll around the corner. In it's current state, I would not be inclined to use comp, even though I prefer it. Comp should give the same toolpath that a CAM program will give. If not, it's a feature that's only partially implemented, imo.

I'm attaching a .pdf I threw together to show what I think it should be.

G41-G42.pdf
(78.9 KiB) Downloaded 109 times



G41/G42 does appear to be working nicely, though, outside of these two issues.
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 Vmax549 » Tue Dec 26, 2017 5:33 pm

I agree with Gerry. The only thing I could add is to allow on inside corners that you be allowed to use the same tool radius or less than the corner radius. This gives teh best tool rigidity for deep pockets. And yes I understand that a tool radius teh same as teh corner radius can somtimes give finish problems but teh Pluses outweight the Minuses in this case

I have been testing in complex subs and so far I AM impressed with UCCNC tool comp.

I would like to see a proper tool table instead of seperate dros (;-) The need for a proper tool table will only geat greater from here on out so now would be a good time to implement it along with G41/42

To add to that teh user MOST understand proper leadin and leadout . You must start teh leadin at least teh tool radius value away from teh start point to give teh machine room to comp that distance. The normal leadin is 2x teh radius or ( Tool Diam). Same with leadout teh machine needs room to uncomp teh distance.

So far so good (;-)

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

Re: G41/G42 discussion.

Postby Vmax549 » Wed Dec 27, 2017 12:05 am

Interesting that even when teh Manual says not to use arcs for leadins/outs they do work.

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

Re: G41/G42 discussion.

Postby ger21 » Wed Dec 27, 2017 2:39 pm

Now would probably be a good time to add wear compensation as well, no? You just add a wear DRO, and add the value to the tool diameter. I personally don't use this, but I know that some do.
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 Vmax549 » Wed Dec 27, 2017 4:47 pm

Here is a glitch. I started at X0Y0Z0 and when I came out of Comp (G40) I was at some unusual position values in the DROs. Seems somewhere it switched over to Machine Coords

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

Re: G41/G42 discussion.

Postby Vmax549 » Wed Dec 27, 2017 6:18 pm

OK Another glitch when using stacked subs and Inc drops in Z. I'll send that example in when you get back from Holiday.

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

Re: G41/G42 discussion.

Postby cncdrive » Wed Dec 27, 2017 8:58 pm

Thanks guys for the feedbacks and I hope everybody had a great Christmas time!

Gerry,

I don't understand point 1. yet, but did not read fully after it yet, I will read the doc you linked to see if I understand what this means and let's discuss it afterwards.

The point 2. is something which we already started implementing. I mean there will be the square shape joints and round joints option for connection angles grater than 180°.
So, it will be an option what you want in point 2., we will finish it in the beginning of January. Unfortunately we could not finish it before Christmas, but wanted to give you guys a release so is why yet only the square joints only are available in this release.

And if you guys find bugs then please post the associated profil file and g-code and some description, because seeing one printscreen is not enough info for us to even start debugging.
It is possible that there are bugs in this version because as I wrote earlier the G41/G42 required serious code changes with additional bufferings, so however we ourselves tested this software version a lot it is possible that some issues remained in which we did not notice.

Terry,

Could you please describe how a proper tool table would look like?
cncdrive
Site Admin
 
Posts: 2187
Joined: Tue Aug 12, 2014 11:17 pm

Re: G41/G42 discussion.

Postby Vmax549 » Wed Dec 27, 2017 9:26 pm

Hi Balazs, Here is where we had talked about it long ago viewtopic.php?f=2&t=320

It would be in a table format linked to teh PRO file. The table would pull all the values out from teh PRO. You would edit the table from inside UCCNC and it would update teh profile automatically.

You could also make it that you could add additional fields to teh table and do sorts on the order you wanted to see displayed.

I have a tool table plugin around here somewhere if I can find it again.


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

Re: G41/G42 discussion.

Postby Vmax549 » Wed Dec 27, 2017 10:04 pm

Hi Balazs, Here is an example code of teh glitch with INC drops in Z . The code as is does an ABS drop of Z for each layer and it works correctly. Edit teh code and you will see teh ABS coding. Comment that out and UNCOMMENT teh INC lines then run teh code and you will see teh glitch. The inc drop of Z gets doubled but in the next 2 move of teh sub it recovers back to teh specified depth of Z.

(;-) TP
Attachments
333.txt
(1.32 KiB) Downloaded 79 times
Vmax549
 
Posts: 1190
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby cncdrive » Wed Dec 27, 2017 11:06 pm

Thanks Terry, I'll debug this soon to see why the issue happens.
I'll also check the thread about the tool table.
cncdrive
Site Admin
 
Posts: 2187
Joined: Tue Aug 12, 2014 11:17 pm

Next

Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: Bing [Bot] and 2 guests