G41/G42 discussion.

[ger21]

I've been using G41/G42 for 20 years making that same exact cut with no issues. 20 years ago on a Masterwood machine with a DOS control, and now with a Morbidelli. There are lots of controls out there that are smart enough to not gouge.

Would this be possible? Say you have round corners enabled. if a segment is shorter than the tool radius, can you switch to square corners for those moves? Not ideal, but better than what it is now. If not, I can work around it.

Why is it that you can look ahead 200 lines for CV, but only 1 line for G41/G42?

[cncdrive]

Hi Gerry,

I will check what can I do about what you adviced about comparing the segment lengh to radius size and switch to square if the check result mets.

There is one line look ahead, because G41/G42 has to work like that.
G41/G42 was developed to make simple codes to offset, so machinists could clearly understand what will exactly happen.
With lots of lines look ahead the operation is not clear, it can't be though out in advance by human.
I did not see any controls so far which would do the calculation differently, but ofcourse I did not see all controls.

And one movement look ahead is a requirement with G41/42, because when you get a new movement you can't complete that movement yet,
because you do not know the point after, so you can't decide yet how to move in. You first have to get the next point, so you can calculate the connection angle and then you know where to move and how to move in.

And maybe I was missunderstandable a bit, but looking ahead more will still not fix this gauging issue.
It does not matter how far you looking ahead this exact code will be still not OK.
What could fix this issue is if a ray-tracking algorithm would be used which looks at the toolpath as a whole, but that is no more a G41/42 algorithm.
And it could require long times to do the calculations. With large codes it can take long minutes to finish the calculation, like how it happens in CAM programs.
I can imagine that some controls implements this, but it requires a prior calculation, you then loose the ability too to change the offset on the fly,
and as said I would not call this a G41/42 anymore, because it does not work as a G41/42, it does the offset calculation, but in a different way as how G41/42 is defined to work.

[ger21]

And it could require long times to do the calculations. With large codes it can take long minutes to finish the calculation, like how it happens in CAM programs.

An offset toolpath in a CAM program, or an offset line in CAD, usually happens instantly. I've never seen a several minute wait.

Sorry, I just don't understand why it's any different. (fortunately I don't need to. )

[cncdrive]

Yes, it happens fast if there are a few lines, but it can happen really slow if there are lots of lines and the path is complex.
Ray tracing works fully different as how G41/42, there is not a single thing the 2 algorithms are common.
G41/42 goes through along the path checking the path vectors through can calculating the offset continously.
So, the algorithm only sees a few lines segments at a time and so it requires low processing time and low memory is required.
Ray tracing loads the whole path in and then it starts placing trace lines to explore where the path boundaries are and constructing an offset path based on what it explored.
The algorithm can be time and memory consuming as the number of vectors grows and the more complex the path is the slower the algorithm becomes.
So, the big difference is that G41/42 algorithm calculates on the fly, ray tracking has to be pre-calculated on the whole path and the calculated path has to be stored and can't be changed on the fly.

[Battwell]

new tool table is looking good in latest version.
hiding the save tooltable on exit option - hidden on apearance page ???

re g41 42 ..
with rounded corners- much closer to how it should work.
just have to sort out the small segment fault now- as with rounded corners option - it now gouges into the job- see pic attatched

[Battwell]

as mentioned by ger- even my old biesse with 1992 software could outline without gouging- but that was a point to point machine- so probably using no look ahead whatsoever. i know it would take ages to make up its mind what to do if it had to do parametric math with tool comp on.
i could lead in from any direction or as an arc to the start point as long as it was over diameter of tool length or more long lead in.
when your programming g41/42 are you working from just the centre of tool or using closest circumference tangents for calculation?

[Battwell]

HI Batwell Could you share teh Gcode for that ? I would like to play with it a bit. I see what appears to be a gouge just before teh leadout ??

(;-) TP

the code was just quickly modified by hand- i didnt care about that bit- just the gouge at the bottom- where a segment gets decreased into a gouge. this segment does get thrown as an error- i ignored it to see if that had been fixed. (fails on all hobby controls ive tried, but- apparently according to one of the lads in uk i shared code with- doesnt gouge on centroid acorn... dont know if thats true- i havnt seen it for myself!

heres the code - ididnt care where the lead in was! set tool 1 diameter to 12mm or 1/2" american
i hadnt even converted it to arcs lol

( g42 )
( File created: Saturday December 23 2017 - 02:41 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 250.000, Y= 125.000 ,Z= 20.000)
()
(Toolpaths used in this file:)
(g42)
(Tools used in this file: )
(13 = End Mill {6 mm})
N100G00G21G17G90G40G49G80
N110G71G91.1
N120T13M06
N130 (End Mill {6 mm})
N140G00G43Z45.720H13
N150S16000M03
N160(Toolpath:- g42)
N170()
N180G94
x-50 y0
g42d1
N190X0.000Y116.000F3600.0
N200G00X2.968Y116.664Z5.000
N210G00X2.968Y116.664Z1.000
N220G1X2.968Y116.664Z-19.000F1200.0
N230G1X89.607Y30.000Z-19.000F3600.0
N240G1X90.356Y30.734Z-19.000
N250G1X91.121Y31.449Z-19.000
N260G1X91.904Y32.144Z-19.000
N270G1X92.703Y32.820Z-19.000
N280G1X93.517Y33.475Z-19.000
N290G1X94.347Y34.111Z-19.000
N300G1X95.193Y34.725Z-19.000
N310G1X96.052Y35.319Z-19.000
N320G1X96.926Y35.892Z-19.000
N330G1X97.814Y36.444Z-19.000
N340G1X98.715Y36.973Z-19.000
N350G1X99.629Y37.481Z-19.000
N360G1X100.556Y37.967Z-19.000
N370G1X101.495Y38.430Z-19.000
N380G1X102.446Y38.870Z-19.000
N390G1X103.409Y39.288Z-19.000
N400G1X104.382Y39.682Z-19.000
N410G1X105.366Y40.053Z-19.000
N420G1X106.360Y40.400Z-19.000
N430G1X107.364Y40.723Z-19.000
N440G1X108.377Y41.022Z-19.000
N450G1X109.399Y41.296Z-19.000
N460G1X110.430Y41.545Z-19.000
N470G1X111.469Y41.769Z-19.000
N480G1X112.516Y41.968Z-19.000
N490G1X113.570Y42.141Z-19.000
N500G1X114.632Y42.288Z-19.000
N510G1X115.700Y42.409Z-19.000
N520G1X116.774Y42.503Z-19.000
N530G1X117.853Y42.571Z-19.000
N540G1X118.938Y42.612Z-19.000
N550G1X120.029Y42.625Z-19.000
N560G1X121.209Y42.609Z-19.000
N570G1X122.381Y42.562Z-19.000
N580G1X123.544Y42.484Z-19.000
N590G1X124.698Y42.377Z-19.000
N600G1X125.841Y42.240Z-19.000
N610G1X126.974Y42.074Z-19.000
N620G1X128.096Y41.881Z-19.000
N630G1X129.206Y41.660Z-19.000
N640G1X130.302Y41.413Z-19.000
N650G1X131.386Y41.140Z-19.000
N660G1X132.455Y40.842Z-19.000
N670G1X133.510Y40.519Z-19.000
N680G1X134.550Y40.172Z-19.000
N690G1X135.573Y39.801Z-19.000
N700G1X136.580Y39.408Z-19.000
N710G1X137.569Y38.993Z-19.000
N720G1X138.541Y38.557Z-19.000
N730G1X139.494Y38.100Z-19.000
N740G1X140.427Y37.623Z-19.000
N750G1X141.341Y37.127Z-19.000
N760G1X142.234Y36.612Z-19.000
N770G1X143.106Y36.078Z-19.000
N780G1X143.956Y35.528Z-19.000
N790G1X144.783Y34.961Z-19.000
N800G1X145.587Y34.377Z-19.000
N810G1X146.367Y33.779Z-19.000
N820G1X147.123Y33.165Z-19.000
N830G1X147.854Y32.537Z-19.000
N840G1X148.558Y31.896Z-19.000
N850G1X149.236Y31.243Z-19.000
N860G1X149.887Y30.577Z-19.000
N870G1X150.510Y29.899Z-19.000
N880G1X172.835Y7.567Z-19.000
N890G1X227.432Y7.604Z-19.000
N900G1X227.432Y4.604Z-19.000
N910G1X244.114Y4.590Z-19.000
N920G1X244.114Y116.664Z-19.000
N930G1X2.968Y116.664Z-19.000
N940G00X2.968Y116.664Z5.000
N950G00Z45.720
N960G00X0.000Y0.000
N970M09
N980M30
%

[Battwell]

again... how many people actually use this feature now.? i mean - in reality ???
as it doesnt work in any of the controls im using now - i have proved i dont need it
however... its a superb bragging right for uccnc software if theirs is the only one that can do it without failing!
i do hear a lot of people saying they wont swap over from mach until its supported- when -already the uccnc version is better than the mach tool radius comp ! - they obviously dont use mach 3 comp!

its so fast to hit recalculate in vectric and re post the code - quicker than doing the math for a different size etc.

i make kitchen cabinet doors for my mate. as long as i have guide lines on in vectric and use mirroring for hinge holes etc i can redo a different size door in a few seconds while one is being cut

[ger21]

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.

[cncdrive]

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.