Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: mannby on December 29, 2005, 04:54:22 PM

Hello,
I got a problem when I use radius compensation, when I load the file Mach complains about:
'Cannot use g28 or g30 with cutter radius comp on line #56'
If I remove G41 and G49 then it works but I can't understand why it wouldn't work with the rad comp.
Please see following code:
// Roger
%
O1
G90 G80 G28 G40 G17
(NOLLPUNKT I INRE VANSTRA HORN UPPE PA BITEN.)
(TOOL 1)
(PINNFRAS TUSA 6MM)
(OPERATION 7)
N1 T1 M6
S9800 M3
G0 X0 Y0
G43 Z3. H1
M8
G0 Z2.5
X130.7468 Y36.3036 Z3.
Z2.5
G1 Z2. F100.0
G41 X131.4302 Y42.2645 D21
G2 X44.4616 Y32.0091 I21.7351 J189.5675 F200.0
X44.4253 Y31.9957 I1.0252 J2.818
X42.4812 Y28.545 I0.9899 J2.8307
G1 X38.0785 Y27.6145
G2 X38.3755 Y26.5817 I7.3367 J1.5505
X33.2157 Y25.4324 I46.3412 J220.2095
X33.1782 Y25.527 I20.5635 J8.0964
G3 X38.0785 Y27.6145 I76.5169 J172.83
G1 X42.4812 Y28.545
G2 X45.9361 Y26.2119 I2.934 J0.62
G3 X131.5177 Y24.6452 I38.7806 J219.8397
G2 X133.4214 Y24.8631 I0.6287 J2.9321
G1 X135.2884 Y29.1499
G3 X136.9862 Y35.934 I27.1152 J3.1817
G1 X138.2203 Y35.7854
G2 X136.4469 Y28.6997 I24.1833 J9.8172
G1 X134.9051 Y23.6031
G2 X135.2476 Y21.0378 I27.4985 J2.3651
X30.0462 Y20.021 I50.5309 J214.6656
X26.9364 Y27.6181 I17.394 J2.685
G3 X136.3859 Y44.3582 I82.7587 J174.9211
G1 X141.6076 Y43.7691
X139.4445 Y41.2862
G2 X137.954 Y38.7736 I22.9591 J15.318
G1 X141.9404 Y36.6857
G2 X142.3008 Y14.589 I20.4632 J10.7175
X25.3426 Y14.0856 I57.5841 J208.2168
X19.074 Y28.754 I12.6904 J3.2504
G3 X151.3828 Y46.2697 I90.6211 J176.057
G2 X141.9404 Y36.6857 I11.0208 J20.3015
G1 X137.954 Y38.7736
G2 X135.3588 Y41.7727 I2.9986 J0.0276
X131.4302 Y42.2645 I25.6637 J189.0757
G0 Z3.
X0 Y0
(TOOL 2)
(PINNFRAS 8MM TUSA)
(OPERATION 8)
M9
G90 G80 G28 G17
G49 G0 Z0 S300 M5
N2 T2 M6
S8000 M3
G0 X11.6522 Y2.664
G43 Z3. H2
M8
G0 Z2.5
G1 Z2. F100.0
G41 Y2.336 D22
G3 X12.6522 Y3.336 I1. J0
G2 I0 J14. F200.0
X13.6514 Y3.3717 I0 J14.
G3 X14.7202 Y2.4456 I0.0713 J0.9975
G1 G40 X15.077 Y2.5417
G0 Z3.
X0 Y0
M9
G90 G80 G28 G17
G49 G0 Z0 S300
M5
G0 X0 Y0
M30
%

Hello,
I got a problem when I use radius compensation, when I load the file Mach complains about:
'Cannot use g28 or g30 with cutter radius comp on line #56'
If I remove G41 and G49 then it works but I can't understand why it wouldn't work with the rad comp.
Please see following code:
// Roger
%
O1
G90 G80 G28 G40 G17
(NOLLPUNKT I INRE VANSTRA HORN UPPE PA BITEN.)
(TOOL 1)
(PINNFRAS TUSA 6MM)
(OPERATION 7)
N1 T1 M6
S9800 M3
G0 X0 Y0
G43 Z3. H1
M8
G0 Z2.5
X130.7468 Y36.3036 Z3.
Z2.5
G1 Z2. F100.0
G41 X131.4302 Y42.2645 D21
G2 X44.4616 Y32.0091 I21.7351 J189.5675 F200.0
X44.4253 Y31.9957 I1.0252 J2.818
X42.4812 Y28.545 I0.9899 J2.8307
G1 X38.0785 Y27.6145
G2 X38.3755 Y26.5817 I7.3367 J1.5505
X33.2157 Y25.4324 I46.3412 J220.2095
X33.1782 Y25.527 I20.5635 J8.0964
G3 X38.0785 Y27.6145 I76.5169 J172.83
G1 X42.4812 Y28.545
G2 X45.9361 Y26.2119 I2.934 J0.62
G3 X131.5177 Y24.6452 I38.7806 J219.8397
G2 X133.4214 Y24.8631 I0.6287 J2.9321
G1 X135.2884 Y29.1499
G3 X136.9862 Y35.934 I27.1152 J3.1817
G1 X138.2203 Y35.7854
G2 X136.4469 Y28.6997 I24.1833 J9.8172
G1 X134.9051 Y23.6031
G2 X135.2476 Y21.0378 I27.4985 J2.3651
X30.0462 Y20.021 I50.5309 J214.6656
X26.9364 Y27.6181 I17.394 J2.685
G3 X136.3859 Y44.3582 I82.7587 J174.9211
G1 X141.6076 Y43.7691
X139.4445 Y41.2862
G2 X137.954 Y38.7736 I22.9591 J15.318
G1 X141.9404 Y36.6857
G2 X142.3008 Y14.589 I20.4632 J10.7175
X25.3426 Y14.0856 I57.5841 J208.2168
X19.074 Y28.754 I12.6904 J3.2504
G3 X151.3828 Y46.2697 I90.6211 J176.057
G2 X141.9404 Y36.6857 I11.0208 J20.3015
G1 X137.954 Y38.7736
G2 X135.3588 Y41.7727 I2.9986 J0.0276
G40 X131.4302 Y42.2645 I25.6637 J189.0757 (added a G40 to this line)
G0 Z3.
X0 Y0
(TOOL 2)
(PINNFRAS 8MM TUSA)
(OPERATION 8)
M9
G90 G80 G28 G17
G49 G0 Z0 S300 M5
N2 T2 M6
S8000 M3
G0 X11.6522 Y2.664
G43 Z3. H2
M8
G0 Z2.5
G1 Z2. F100.0
G41 Y2.336 D22
G3 X12.6522 Y3.336 I1. J0
G2 I0 J14. F200.0
X13.6514 Y3.3717 I0 J14.
G3 X14.7202 Y2.4456 I0.0713 J0.9975
G1 G40 X15.077 Y2.5417
G0 Z3.
X0 Y0
M9
G90 G80 G28 G17
G49 G0 Z0 S300
M5
G0 X0 Y0
M30
%
PLease look at the line I added the G40 to and see if that hepls it

Thanks again Brian,
I will try that tonight. I'm not sure why my post processor didn't put in G40 at that line
because it did at the second operation.
Maybe because the radius compensation continued on the second operation. ???
I will check if I can change the post processor to always put in a G40.
Roger

Hi, now I got the G41 and G40 to work as it should, but when I tried to use the compensation by changing
the tool wear in the tool table nothing happens.
I was trying the following code posted from my cam program:
(TOOL 3)
(MILL 12MM)
(OPERATION 3)
X159.9999 Y4.
G1 Z4. F100.0
G41 Y9. D23
G3 X164.9999 Y14. I5. J0
G2 I0 J21. F200.0
I0 J21.
X165.9995 Y14.0238 I0 J21.
G3 X171.2318 Y9.2675 I0.238 J4.9944
G1 G40 X171.4698 Y4.2731
G0 Z3.
The postprocessor added D23 for tool 3 is that wrong? must the D value be the same as
the tool number?
/Roger

Well I run Fanuc by day so I can tell you why the heck this would ever be the right thing to do:) In a fanuc (but not all) the tool comps pull from memory locations NOT a table. So if you have a 20 tool changer, 120 are all tool length comp and 2140 are dia. This is not a set rule it is just how most people do it.
You don't need know this to run Mach3 :) in Mach3 it is in a table so you only need to do H3 and D3. Please change the post and I think you will be good to go.

Yes your right Brian I was using Fanuc 6 post and now I removed the D value completly.
According to the manual Mach uses the cutter comp slected tool if theres no D value, right?
And does Mach use the tool diameter in the tool table in any way, for ex. in cutter comp?
Roger

You can use the auto d = tool that you have in thing... That should work!
"And does Mach use the tool diameter in the tool table in any way, for ex. in cutter comp?...."
I think you are asking if this is what it is going to get for a val? You are correct
PS the other thing you can do is :
G41 P.125 for a .25 Mill this will make it so you don't need to set anything in the tool table :)
Hope that helps

Brian you wrote "You can use the auto d = tool that you have in thing... "
is that in mach or in the postprocessor?
About the tool table I understand the tool lenght and wear but does it matter
what I type in tool diameter column?
Roger

Brian you wrote "You can use the auto d = tool that you have in mach3... "
is that in mach or in the postprocessor?
About the tool table I understand the tool lenght and wear but does it matter
what I type in tool diameter column?
Roger
Sorry about the the mouse on the computer I was on jumps around and I edn up with words in strange places at times....
The auto D Val is in Mach3
As for the tool table you only need to have the Dia of the tool IF you are going to call it with a G41 or G42.
Hope that helps
Brian

Sorry Brian, I can't find the "Auto d val" in Mach.
Can you tell me where to find it please?
Thanks
Roger

Sorry that was my poor atampt at telling you that if you put nothing Mach will put in the D Val for the T number that is loaded.
Sorry again