Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: RChadwick on August 07, 2008, 12:02:51 PM
-
I've seen this mentioned before, but I still can't quite figure it out...
I'm trying to make a simple 2D cutout in Plexiglas. It's one continuous cut, and looks a little like an F. To get it cut to a precise size, I obviously have to compensate for the end mill diameter. On the main screen of Mach3, there is a tool diameter setting, but putting the diameter in didn't make any difference. I also noticed a setting in Lazycam, which seemed even more thorough (Like asking whether to trace on the inside or outside), but that didn't seem to make a difference either. What I really need is a Tool Diameter Compensation FAQ.
1) Is it better to do this in LazyCAM, or Mach3? Does it need to be done in both? All things being equal, I'd rather do it in Mach3, as I likely will decide on different size tools.
2) Is there an accurate way to predict the cut will be right? The part I'm making is 1 inch long, using a cutter less than 1MM Dia.
3) Some of the areas between larger protrusions (Think of the area between the top and middle protrusion on the letter F) are only slightly larger than the end mill. Will this confuse Mach3?
-
Cutter diameter compensation is governed by G40 (Compensation off) G41 (Compensation left) and G42 (Compensation right). What I must admit is that I have never been told what left and right mean - does that mean the tool is on the left or right - or the compensation is on the left or right.
In the case of the enclosed "window" - do you have to change as the cutter goes up one side, then down the other. I do not know. Perhaps someone versed in G Code could tell us. However I have no doubt that Mach does it correctly.
When cutting something like this, I have always written the code to cut, i.e. where I want the tool to go, and you can look at the code and check it before cutting, especially if your tolerances are so fine (a cutter less than a mm - phew).
There is another problem as well - where the cut finishes. Start the cut halfway along a straight edge and finish along the same straight edge, do not meet at a corner - because you do not know where the compensation is applied.
I hope you understand the diatribe - and perhaps spmeone will enlighten us.
-
I appreciate the response. However, G-Code is like Greek to me :). It's well beyond my abilities to write G-Code for even the existing shape, let alone compensating for the tool. I was hoping this was something that could be automatically calculated by Lazycam or Mach3. I probably should have prefaced my original comment by saying that I am a complete CNC newbie. I have made only 2 things in my life on a CNC machine (Which I'm actually very impressed I made it this far), and neither turned out right because the tool followed the outline of the object without compensating for tool diameter.
-
What I must admit is that I have never been told what left and right mean - does that mean the tool is on the left or right - or the compensation is on the left or right.
Actually, those are both the same. :) Comp right would be to move the tool right.
There is another problem as well - where the cut finishes. Start the cut halfway along a straight edge and finish along the same straight edge, do not meet at a corner - because you do not know where the compensation is applied.
If you lift the tool before calling G40, you don't have to worry about it.
I think the OP needs a CAM package to do the offsets for him. V-Carve Pro and I believe SheetCAM will both do this. Does LazyCAM Pro do it as well?
-
Hi, As far as I understand, and please correct me if I am wrong!! The compensation follows the direction of the cutter ie: If you were cutting a square shape in a clockwise direction and you wanted the end result to be a square hole the cutter should be offset to the right, If you wanted the result to be a solid square in the middle you would use left compensation. It is only when you change direction eg: going anticlockwise that you need to alter the offset to the left. like if you were to cut an S shape you would need both left and right tool compensation. I have seen on the forum that if you have to change from left to right it is best to move the cutter out of the material before changing offsets.
I would have thought it was best to set the value of offset in Mach rather than in the code so if you have to change cutters and your second cutter has been reground ie slightly smaller in diameter, it will make it easier to get the final result perfect.
Am I making sense or have I had one too many..
-
As I remember from the little I've used tool diameter compensation you have to enter the tool diameters into mach's tool table, i.e T1 = 1mm etc.
you then call T1 in your code move to position then call the appropriate compensation G41 or G42, you then cancel the compensation after the tool is out of the job at the safe height.
Do a search on google for G40, 41 and 42
I also seem to remember there being a problem Mach at some point with calling compensation before the first move.
Steve
-
You don't need to set up the tool table to use comp, but you can if you like. There are two ways to use it. (Actually 3)
1) Call comp and specify the tool radius using the P word. For a 1/8" diameter bit, you'd use G41 P0.0625 or G42 P0.0625.
2) Call comp and specify the tool # in the tool table using the D word. This will use the radius of the tool in the table. To use comp with tool #3, use G41 D3 or G42 D3.
3) Basically the same as #2, but don't call any tool at all. Mach3 will use the diameter of the current tool (based on the diameter in the tool table). Just use G41 or G42.
To use comp properly, you need a lead in move where the comp is applied. Without comp, the center of the tool follows the g-code. When you call G41/G42, comp is applied during the move from the previous location to the one following the G41/G42. I like to use G41/G42 on it's own line, but you can combine it with the leadin move. Both of these will do the same thing:
G1 X0 Y0
G42 D1
G1 X1 Y1
G1 X2 Y1
is the same as
G1 X0 Y0
G1 G42 D1 X1 Y1
G1 X2 Y1
Once comp is applied, it remains in effect until you call G40. Depending on the move following the G40, comp can be either gradually or abruptly removed. You can use a leadout move, or you can raise the tool above the work and then remove the comp.
Left(G41) or right (G42) is pretty easy to figure out. Imagine walking along the toolpath in the cut direction. G42 will move the tool to the right side of the path, G41 will move it to the left side of the path. If you have a circular CCW toolpath, G42 will cut outside the toolpath, G41 will cut inside the toolpath. One thing that can be tricky is climb vs conventional cutting. Which method you're using will dictate whether you need G41/G42, as it determines the direction of the toolpath. The circular example above is using conventional cutting
Here's a little sample program that will show you how it works.
G40
M3
G0 Z0.1250
G0 X1.4629 Y1.2013 Z0.1250
G1 X1.4629 Y1.2013 Z0.0000 F25
G42P0.25
G1 X2.6956 Y2.0815 Z-0.2500 F50
G1 X8.2664 Y2.0815 Z-0.2500
G1 X8.2664 Y6.2744 Z-0.2500
G1 X3.4479 Y6.2744 Z-0.2500
G1 X3.4479 Y1.5214 Z-0.2500
G40
G1 X2.8556 Y0.9132 Z-0.2500
G0 X2.8556 Y0.9132 Z0.1250
G0 X0 Y0
M5
M30
-
RChadwick,
1mm is a small endmill and it won't take much to snap it off when plunging or cutting. I use 1/32" (.031 dia and even 1/64") in my engraving machine and as you know they are not cheap. Keep depth cuts approx equal to 1/2 the diameter or less keeping chips out of the cutter path, better yet, experiment with an 1/8 end mill to gain some experience on the plexiglass ( goes for some of the other plastics also). Plexiglass is a pain to cut, it will wrap around that little bit and break it in a heartbeat. Need to keep the cutting cool using water, cold air gun, cutting fluid, to name a few.
When in doubt on how things will cut you can always dry run a program with a tooth pick in the chuck. They are cheap!
Have made a spring loaded tracer which uses ball point refills for checking out a pattern on paper.
Just a few things to think about.
RICH
-
Thanks for the comments Rich. I realize it's a very small end mill. Although I expected problems, my first one snapped almost immediately. I slowed the feed rate to next to nothing, and I managed to not snap them so often .Then, it was melting the plexiglas, making a mess. I solved that by making a clay lip around the work area, and filling it with water. I actually managed to get a decent quality cut. If anything, I'll need a smaller end mill to get the detail I'll probably need. I bought a few of those cheapie resharpened carbide cutters/drills available nearly everywhere, and it eases the emotional pain when they break :)
My biggest problem now, and likely my last hurdle, is to get Mach3 to take into account the diameter of the cutter, and have it go around the outside of the lines. I've taken a vacation from it tonight :)
-
It might be a bit late in the day (or the year, or in life) to try and get you interested in G Code, but it is very simple. The only trouble is that CAM programs write masses of it because they are so simple.
Each line of code is a move. All commands on a line are done simultaneously.
There are only two moves - G0 which is move fast - and G1 - which is move as fast as I tell you with the F command. There are other cutting moves, but I doubt your CAM program will do them - G2 and G3 - which cut circles.
If you are doing a shape - and you say you did one once - then you must know its dimensions. If you take the trouble to look at your GCode, and lay it out on graph paper, you will see the cuts follow, from one to the other, and all the GCode is telling the machine is where to go next (X and Y) and how high the cutter has to be (Z).
I take it you are using millimeters. So if your first cut is (starting at 0,0) G1 F5 X5, then the cutter is going to move to X5 - along the Y axis. Now if tool diameter compensation is applied by the cam - say for a 1mm cutter - then the Y axis must move from 0 to 0.5 first, and any subsequent moves will also be 1/2 milimeter offset or the inside of the shape if it is a pocket, or the outside if it is an island.
I am not suggesting that you now become a GCode buff - but have a look at the code and try to understand it a little. You will be suprised at how much you can decipher. All the umpteen other moves are to get the cutter to the right place to begin cutting and the only ones that mean anything at all are the G0 and G1.
You will see from the other answers that a lot of people are not certain how tool diameter compensation works - we could do with a comment from Graham Waterworth if he reads this - or pop a question on the GCode forum - and he might see it. He certainly knows his stuff.
-
So I take it tool diameter compensation has to be done before Mach3? Will LazyCam do this perhaps? It's not that I'm terribly afraid of G Code, it's that it would be much more efficient for me to simply change a parameter when I need to try a different tool, instead of opening an editor, remembering what I'm supposed to do, make the changes, and hope I didn't make a mistake.
-
So I take it tool diameter compensation has to be done before Mach3?
The G-code needs the G41/G42/G40 in it, and must be coded correctly to allow for the lead in. But if you use G42 Dx, then all you'll ned to do is change the tool diameter in the tool table to make adjustments for tool size.
-
Yes Gerry -
We understand the pros and cons - but what we need is someone who can properly explain G41 and G42 to us - i.e. comp left and right etc. - for example if you are cutting a window with the tool on the inside, which with standard bit rotation would probably mean you are cutting round in a clockwise direction, what do you use, and for example (since it says left and right) do you need to alter it when you come down the other side)???
-
Hi, Imagine the cutter is a car with 2 steering wheels, one on the left for turning left and one on the right for turning right.
OK so far.
So you get in your car on the right hand side and drive. You can only turn right hand turns so, eventually if you turn 4 rights you have travelled in a rectangle or square. Which ever compensation you used, right for a hole, left for an island. You did not need to change it.
Now lets say the road is an S shape. The start of the S is a left hand turn so jump over to the left seat of the car and start driving left. You follow the S road until you get to the middle of the S you will see that you will need to turn to the right. To do this you have to stop the car and jump into the right hand seat to turn right.
The point at which you have to jump over to the correct seat in the car is the point at which you need to change the cutter compensation if you want to keep following the correct cutter path.
If you were actually cutting an S in material and you had only left compensation on, the bottom of the S would follow the correct path but the top part would not.
John
-
Hi, Imagine the cutter is a car with 2 steering wheels, one on the left for turning left and one on the right for turning right.
OK so far.
So you get in your car on the right hand side and drive. You can only turn right hand turns so, eventually if you turn 4 rights you have travelled in a rectangle or square. Which ever compensation you used, right for a hole, left for an island. You did not need to change it.
Now lets say the road is an S shape. The start of the S is a left hand turn so jump over to the left seat of the car and start driving left. You follow the S road until you get to the middle of the S you will see that you will need to turn to the right. To do this you have to stop the car and jump into the right hand seat to turn right.
The point at which you have to jump over to the correct seat in the car is the point at which you need to change the cutter compensation if you want to keep following the correct cutter path.
If you were actually cutting an S in material and you had only left compensation on, the bottom of the S would follow the correct path but the top part would not.
John
I thought I already explained it in one of my previous posts.
But in regards to following an S shape, you do NOT switch from left to right comp. If you are cutting out a letter S, you use the same comp, all the way around. You use Left or right depending on whether you want to climb cut or conventional cut.
Think of driving down a two lane road, and the center line is the toolpath. G42 is driving on the American side, G41 is driving on the British side. Changing the comp would cause you to cross the line. You never switch comp direction in the middle of a cut. If you drive along an S shaped road, you don't cross the center line when you switch from turning right to turning left, do you?
-
Duh, So I'm another one that's got it wrong!
I think I'll stay as confused as everyone else.
-
- for example if you are cutting a window with the tool on the inside, which with standard bit rotation would probably mean you are cutting round in a clockwise direction, what do you use, and for example (since it says left and right) do you need to alter it when you come down the other side)???
Again, I explained it in my previous post, and offered an example for cutting around the outside. Here's one for the inside.
G40
M3
G0 Z0.1250
G0 X0.6391 Y0.7309 Z0.1250
G1 X0.6391 Y0.7309 Z-0.2500 F50
G42P0.25
G1 X0.0000 Y1.5000 Z-0.2500 F150
G1 X0.0000 Y3.0000 Z-0.2500
G1 X3.0000 Y3.0000 Z-0.2500
G1 X3.0000 Y0.0000 Z-0.2500
G1 X0.0000 Y0.0000 Z-0.2500
G1 X0.0000 Y1.9312 Z-0.2500
G40
G1 X0.5000 Y1.9312 Z-0.2500
G0 X0.5000 Y1.9312 Z0.1250
G0 X0 Y0
M5
M30
-
Here's an S.
G40
M3
G0 Z0.1250
G0 X1.5603 Y4.3285 Z0.1250
G1 X1.5603 Y4.3285 Z-0.1000 F50
G42P0.0625
G1 X1.1250 Y4.2500 Z-0.1000 F150
G3 X1.1250 Y2.0000 Z-0.1000 I0.0000 J-1.1250
G2 X1.1250 Y0.2500 Z-0.1000 I0.0000 J-0.8750
G3 X1.1250 Y0.0000 Z-0.1000 I0.0000 J-0.1250
G3 X1.1250 Y2.2500 Z-0.1000 I0.0000 J1.1250
G2 X1.1250 Y4.0000 Z-0.1000 I0.0000 J0.8750
G3 X1.1250 Y4.2500 Z-0.1000 I0.0000 J0.1250
G2 X1.0000 Y4.3750 Z-0.1000 I0.0000 J0.1250
G40
G1 X1.0000 Y4.6250 Z-0.1000
G0 X1.0000 Y4.6250 Z0.1250
G0 X0 Y0
M5
M30
-
As Gerry has said one is for going down the left of the line (tool path) as you look in the direction of travel (g41) the other is for going down the right of the line as you look in the direction of travel (g42)
You can can also lie to it to alter the offset in relation to the size of the cutter to get a larger or smaller part (or hole)
G41 also climb cuts while G42 is conventional cutting.
So if your machine has a significant amount of backlash then always use G42 and go Anti clockwise to cut on the outside and clockwise to cut on the inside.
I tend to use a CAM program though as it sorts it all out for you and it always says in the code what size cutter was used.
Steve
-
I am at a loss at to why a tool number is even called with a D word. Why not just use the currently called tool number? That is the standard way of doing it, right? If there is indeed a reason for the D word, please tell. I know I was at a loss trying to use comp without the D word. In 99% of my projects, tool comp is applied inside the cam program, not at the control. However, there are times when needed at the control.
3) Basically the same as #2, but don't call any tool at all. Mach3 will use the diameter of the current tool (based on the diameter in the tool table). Just use G41 or G42.
Don't seem to work for me. Never has. Maybe I'm just doing something wrong. Maybe this has been giving other people trouble as well.
If I load Mach from scratch, and load this program, tool comp is NOT applied.
g90g20g61t1f1000
g01x-0.5y-0.5
g01g42x0.0y0.0
x2.0y0.0
x2.0y2.0
x0.0y2.0
x0.0y0.0
x2.0y0.0
g01g40x2.5y-0.5
m30
If I insert a D value, toll comp IS applied. For instance if I change the first line to....
g90g20g61t1d1f1000
or
g90g20g61d1f1000
(whichever one you prefer, pick your poison)
now....stay with me here...if you edit the code AGAIN, back to the original way it was, (without the D value, and only a T call) tool comp magically works, and I can modify the value in the tool table, and MACH will indeed account for those changes.
So, in short..... If you use code without a D value, a tool call alone will not work. If you ADD a D value, and then remove it, a tool call alone WILL work. Strange indeed.
-
I have been asked to try and clarify the cutter compensation debate (CC) that keeps raging on and on and on.........
The basics
Compensation is not a quick fix.
Cutter compensation is used to adjust the size of a cut area, this can be on the outside or the inside of a component or section of a component.
Compensation has to be planned into the job, it is not easy to adapt afterwards.
When programming the job the tool is programmed on the centre line of the cut.
When programming the part any inside radius can not be smaller than the radius of the cutter to be used.
The machine should never rapid with an active G41 or G42, Mach3 may allow this move just as you can drive your car off a cliff, its not advisable.
You should not change local (G52) or global (G54-G59 Etc.) work offsets while a G41 or G42 is active.
Cutter compensation should not be used for pocketing and area clearance.
How it works
To use CC we have to command a G41 or a G42, the one we use depends on which side of the line we are on and what direction we want to travel. The next consideration is how we move onto the cutter path, we can not rapid straight onto the line and start cutting, we have to create a lead in line. We also have to have lead out lines. This is why you have to pre-plan CC.
A lead line can be a straight line or an arc or a combination of both. Straight line moves are the easiest, arcs give the best blend.
The picture below shows 4 examples of how we can use CC, the top 2 show cutting on the outside of the green line. The bottom two are slots so are cutting on the inside of the green line.
The parts are 10mm wide and 50mm long giving 40 mm centres on the rads. The example code was written for the use of a 2mm dia end mill. Before anybody tells me this is not the best cutter for the job, I don't care.
More later........
Graham.
%
G54 G00 G90 G43
T1 M6
S1500 M3
(FIG 1 - CCW INSIDE)
G00 X41.5 Y-2.5
G00 Z1.
G01 Z-2. F900.
G41 X42.5 Y2.5 F1800.
G03 X40. Y5. R2.5
G01 X0.
G03 X-5. Y0. R5.
X0. Y-5. R5.
G01 X40.
G03 X45. Y0. R5.
X40. Y5. R5.
X37.5 Y2.5 R2.5
G01 G40 X38.5 Y-2.5
G00 Z25.
(FIG 2 - CW INSIDE)
G00 X61.713 Y-2.5
Z1.
G01 Z-2. F900.
G42 X60.713 Y2.5 F1800.
G02 X63.213 Y5. R2.5
G01 X100.
G02 X105. Y0. R5.
X100. Y-5. R5.
G01 X60.
G02 X55. Y0. R5.
X60. Y5. R5.
G01 X63.213
G02 X65.713 Y2.5 R2.5
G01 G40 X64.713 Y-2.5
G00 Z25.
(FIG 3 - CCW OUTSIDE)
G00 X41.5 Y42.5
Z1.
G01 Z-2. F900.
G42 X42.5 Y37.5 F1800.
G02 X40. Y35. R2.5
G01 X0.
G03 X-5. Y30. R5.
X0. Y25. R5.
G01 X40.
G03 X45. Y30. R5.
X40. Y35. R5.
G02 X37.5 Y37.5 R2.5
G01 G40 X38.5 Y42.5
G00 Z25.
(FIG 4 - CW OUTSIDE)
G00 X61.074 Y42.5
Z1.
G01 Z-2. F900.
G41 X60.074 Y37.5 F1800.
G03 X62.574 Y35. R2.5
G01 X100.
G02 X105. Y30. R5.
X100. Y25. R5.
G01 X60.
G02 X55. Y30. R5.
X60. Y35. R5.
G01 X62.574
G03 X65.074 Y37.5 R2.5
G01 G40 X64.074 Y42.5
G00 Z25.
G91 G28 Y0 Z0
M30
%
-
I am at a loss at to why a tool number is even called with a D word. Why not just use the currently called tool number?
Sam,
The 'D' in tool compensation has many uses, as a quick example:-
If you had to rough and finish the outside of a stainless steel part you could use a main program to call a sub program of the finished shape and by using 2 different D's you could use the same sub with 2 different sized tools.
Graham.
-
you could use the same sub with 2 different sized tools.
I see. Thank you. I can think of more than once that would have come in handy.
-
If I load Mach from scratch, and load this program, tool comp is NOT applied.
g90g20g61t1f1000
g01x-0.5y-0.5
g01g42x0.0y0.0
x2.0y0.0
x2.0y2.0
x0.0y2.0
x0.0y0.0
x2.0y0.0
g01g40x2.5y-0.5
m30
When you first start Mach3, the current tool is tool 0, which is probably why it doesn't work.
-
Your absolutely correct, Gerry. I didn't complete the tool call using M6, so it remained at tool 0. Goes to show how much manual coding I do. Good catch.
-
hi sid
i havent read all the posts on this topic so someone may have already explained this better but i have a reasonable understanding of cutter
compensation ie left or right.
basically it relates to cutter direction in relation to the programmed path. for G41 (left) the tool will CLIMB mill and for G42 (right) the tool will conventional mill
to put this clearer - if you want to cut the outside of a circle in a clockwise motion use G41
- if you want to cut the outside of a circle in an anticlockwise motion use G42
another way to look at it is if you look at the cutter as it cuts away from you , the cutter compensation will put the on either the left or the right of the programmed path. LEFT (G41) for left ect ect
as far as actually calling it up in mach3 i dont know yet. im a newby myself
hope i helped
-
While I appreciate all the G Code info (It encouraged me to dig in a little deeper), I have been a little confused as to why nobody told me how to do it in Lazycam. I think I might have just answered my own question. While this is probably obvious to everyone, it took me a little while to figure out the unregistered, non-pro version of lazycam apparently doesn't do tool compensation. I tried adding the appropriate G-codes, but I must not have gotten the syntax right. Can anyone tell me if it's worth it to buy the registered version? I'm a little nervous, it being in beta still, with no instructions.
-
RCHADWICK,
"Can anyone tell me if it's worth it to buy the registered version?"
I can only speak for myself. I use it mainly for the lathe and still learning for the mill. My answer would be yes for a few reasons.
1. Where alse are you going to get a program like that for what your going to pay?
It's Beta? Hell, I beta'd for five years with one particular program and frankly I think 10 years from now you will
still be "beta-ing" with any program because nothing stands still.
2. Where else are you going to get the kind of support provided by realy nice knowledgable people?
May I add that some do it for a living so will add professional to the people discription.
3. Where else would someone spend the time to explain what you just picked up from this thread?
4. Where alse can you get someone to stay by your side, have you in their thoughts, until you arrived at an end of a
problem in trying to do or learn something?
5. Some programs require more that what you pay for it just as a yearly support fee and addtionaly you should end up
getting upgrade for free.
6. Sooner or later you will want to do or try something complex and you will appreciate that program.
Again, just something to think about.
RICH
-
Not used lazycam but if it works like most other cam programs then it doesn't use cutter compensation.
You tell the cam program the process needed (inside, outside, left, right) and the tool size and the program works out the rest and outputs code for the centre line of the cutter so you have to use that size cutter to cut the job.
Sheetcam can add or remove an amount set in the process dialog so you can leave a small amount for a finishing cut etc, non of this uses G41/42 but seems to off set the original lines.
Years ago when I was using CNC for work we used to have to hand code so we always wrote the code for the centre line of the job and then applied tool compensation.
Now I don't use it, I just send the job through my cam program with a different cutter if I have to change it.
Steve
-
While I appreciate all the G Code info (It encouraged me to dig in a little deeper), I have been a little confused as to why nobody told me how to do it in Lazycam.
Don't use it.
-
Don't use Lazycam?
-
Don't use Lazycam?
He means he doesn't use LazyCAM so thats why he didnt tell you how to do it with LazyCAM ;)
Hood
-
:)
-
Yep, don't use LazyCAM. ;)
-
Just reading through this post on cutter comp, Graham says g41 or g42 on a lead in (g1 or g2-g3)-( Correct me if I'm wrong,) but I was always taught
Not to use cc on a lead in arc. Always g41 or g42 on a linar (g1) move first, than the arc. example-g41 x0y0 than g2 or g3 for your blend. Then when you arc out for
blend-g40 with no g1. I always make my lead in g1 no less than my cutter di.
Thats the way I always do it.
Ed V,
-
Hi Ed,
your comments are true, but it also depends on the control some need 90 degree only approach others can work out vectoring some will apply the the cc during the rapid to position. If you read through the G-code examples you will find that the samples are code as you were taught. CC can also be applied on a single arc lead in.
Graham.
-
Thanks Graham,
So, if cc works in a rapid to position, this would cut down the machining time, which is a good thing.
I'll have to try more variables,
Ed V.
-
I'll have to try more variables,
Ed V.
I am sure you already have, I mean being married to Bretts sister must hold vast quantities of variables ;D
Hood
-
And she learned them all from Brett. ;D
-
I can imagine ;D
On second thoughts I think I would rather NOT imagine ;)
Hood
-
hi ,
i am using mach3mill latest version R3.043.067.
1)when tool compensation g41 or g42 is used the inner circle dosent seem to close when i stimulate & also run it online using machine.
i have attached the g code and screen short of the eg files.
g code program is made for the corresponding size.
[sq size 50x50 with fillet 5mm and inner 20mm dia circle].
need help .please clarify
regards
adhityanpt
india
-
Can you attach your xml file.
Just tried the iner one and works here.
RICH
-
I see the same problem testing in V.067.
(;-) TP