[armandon]

I'm trying to cut a rectangle as shown in blue (tool diam. 2mm), with the code shown below. But the result I get is shown in red.
Any help is welcome, thanks in advance.

[IMG]file:///D:/consultaCNC.gif[/IMG]


%
G90 G21 G17
G40 G49
G00 X 5.00 Y 20.00 Z 2.00 F200
G41 P1.0
G00 X 6.80 Y 27.000
G01 Z -2.00
G01 X 31.00 Y 27.00
G01 X 31.00 Y 37.00
G01 X 6.80 Y 37.00
G01 X 6.80 Y 27.00
G00 Z 2.00
G40
M30

[ger21]

Can't see the pic, but try this. I don't have Mach3 here, so I can't test it.


%
G90 G21 G17
G40 G49
G00 X 5.00 Y 20.00 Z 2.00 F200
G00 X 6.80 Y 22.00
G41 P1.0
G01 X6.80 Y26 Z -2.00
G01 X 31.00 Y 27.00
G01 X 31.00 Y 37.00
G01 X 6.80 Y 37.00
G01 X 6.80 Y 26.00
G00 Z 2.00
G40
M30

[armandon]

Gerry, thank for your response.

In the attached files are the graphics with the trayectories with the old and the modified code.

The tool should down in the coordinates (7.80, 28.00) but no ....

I can't to use the line

G01 X6.80 Y26 Z -2.00

the tool down progressively with the X motion.I think it should be separated into two blocks.

G01 Z -2.00
G01 X6.80 Y26

Best regards

[ger21]

I can't to use the line

G01 X6.80 Y26 Z -2.00

the tool down progressively with the X motion.I think it should be separated into two blocks.

I always do that, to ramp into the cut. It's much better for your tools.

Now that I'm looking at it, I see that I made a mistake before.
I think that you want to use G42, to be on the outside of the cut??

Like this"



G90 G21 G17
G40 G49
G00 X 3.00 Y 20.00 Z 2.00 F200
G00 X 5 Y 27.00
G42 P1.0
G01 X6.80 Y27 Z -2.00
G01 X 31.00 Y 27.00
G01 X 31.00 Y 37.00
G01 X 6.80 Y 37.00
G01 X 6.80 Y 26.00
G00 Z 2.00
G40
M30

[mactec54]

armandon

You have to give the G41 or G42 a feed move before it will be active the same to cancel
A link that shows how to make cutter comp work

Cutter Compensation Example

Yes you should have a Z safe move before a G0 X, Y move

[armandon]

Thank Gerry, Mactec54

Improved my question.
I need to cut a rectangular window in an plastic enclosure as show in blue. The tool path that I tried to follow is shown in red (with the code posted), but the results obtained are the shown in the figure of prev post.

Is posible that are some parameters bad configurated in Mach3 ?

regards

[ger21]

This should work for you.

G90 G21 G17
G40 G49
G00 X15.00 Y29.00 Z2.00 F200
G00 Z0
G41 P1.0
G01 X20.00 Y27 Z -2.00
G01 X31.00 Y27.00
G01 X31.00 Y37.00
G01 X6.80 Y37.00
G01 X6.80 Y27.00
G01 X22.00 Y27.00
G01 X25.00 Y29.00 Z0
G40
G00 Z2.00
M30

[mactec54]

armandon

Using the ( P1 ) word will turn any tool comp you have for that tool ( OFF )

To have it read the tool size you put in the offset should be ( D1 ) if you want it active

G41X___D1 You need to do a straight move to turn the cutter comp on, so start 10mm away from were you want to start cutting & then it will work, You should also do a straight move off the part to turn it off

[ger21]

Mactec, G41 P1 offsets the tool 1mm. Which appears to be what he wants, looking at the last image he posted.

[armandon]

Gerry, the code posted works fine.

Mactec54, I'll test your suggestions.

Thank you very much to both for your help !

Can you recomend an G-Code tutorial or book ?

Thank again !

[mactec54]

ger21


Cutter compensation is used to offset the tool path by the amount specified by the current diameter offset number. The diameter offset is usually specified with a tool change as a D followed by the offset. The offset can be the diameter of the tool, but it can also be used to specify a smaller offset to account for smaller tool size due to wear.

G41 Cutter Compensation Left

Cutter compensation is initialized by a linear move to the specified location. The material is to the left side of the tool as it follows the path.

In normal use of cutter comp no letter P or D is not needed But D is used for this if needed

This is all that is needed to turn it on G41G1X__ F10.& what offset you have in the tool table will be active for the cutter in use

The P word can be used like you have, But you can not ajust the tool off set in the control when using the P word

[mactec54]

armandon

Just Google G codes or the G code you want to learn about, & you will find everthing you need

[ger21]

Thanks, but I know how it works. I've been using it daily for about 15 years.

You said using P turns comp off. I said it didn't. ???

In normal use of cutter comp no letter P or D is not needed But D is used for this if needed

You have to be careful here. With Mach3, the default tool is tool 0, so if you don't do a tool change, you won't get an offset.

[mactec54]

ger21

You said using P turns comp off. I said it didn't. ???

So you are saying the Mach documents are wrong

G41/G42 can be used with the P-word, this will override the value of the tool diameter that is set in the tool table so you can not ajust the offset in the control when using the P-word

[Al_The_Man]

Can you recomend an G-Code tutorial or book ?

One definitive book is CNC Programming Handbook by Peter Smid.
Al.

[ger21]

Never mind, I misunderstood what you were saying. After reading it for the 4th time, I get it.

The manual uses a better choice of words, imo.

G41 and G42 can be qualified by a P-word. This will override the value of the diameter of the tool (if any) given in the current tool table entry.