Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: softselect on January 01, 2008, 02:17:42 PM
-
Hi everyone,
Happy new year.
I have just completed setting up my lathe with Mach3 v3.0
I have got the CSS sorted with the index pulse, works well.
I have a quick change tool holder. (infact 2 in front and 1 at the back)
I have setup the tools in G53
when I run my program the tool number stays on 0, enven though it asks for tool change.
Please help
-
You need to put the tools in the format of Tool number then Tool offset
So it would be like T0101 for tool 1 offset 1 or T0102 for tool 1 Offset 2.
You can miss out the 0 at the start and have eg T101
Hood
-
Thanks Hood, it works but it doesnt.
I get the maching moving very slowly to some weard position after tool change.
the Offsets are correct because when i manually change the tool in the tool number window and MDI a position it goes to the correct position. eg X50,Z50
I may have something wrong in my NC file could you please take a look for me
Thanks Freidrich
PS in may be due to the fact that i am using G95
-
try it without the G0 infront of the T202
Hood
-
Hi Hood,
I did in the first place , then I put g00 in front thinking it would force modal g00
with G00 or without it creeps to some weard position
I think if the rest of the setup is ok, I will try changing to G94 and addapt the speeds and feeds and see what it does.
does the tip dir have to be setup, my path is cad generated so it precompensates for tip rad.
Thanks Friedrich
-
Might be worth trying the G94 before the toolchange and then G95 after, you could probably edit your Post Processor to do that for you when a toolchange is called for. I am not great with code so take what I say with a pinch of salt, Graham Waterworth is your guy for that.
Nope if its CAM generated no tip dir or radius needed.
Hood
-
hi Hood,
still no luck, i setup the tools as in the manual, in program coords, the macine cords are the same when i go to them,
when the program runs, i dont know where i am, i put in G53 or G54 and it makes no diffs, i still get this slow moving to some strange position.
maybe I am not setting the tools up correctly, but why would it work in manual mode when i select toolnumber and move to a coord its, correct.
in manual mode when i call a tool the coord display changes to the new position but the axis stands still, this is correct, so why do the aixs move under auto mode?
(I have a Harding cnc with a NUM control on it. so i understang the consept)
-
At the end of each tool, after it rapids to tool change position insert Tnn00, this cancels the last tool offset. nn is the tool number in use.
There are a few bugs it turn, this may be one of them.
Graham.
-
Hi Graham,
thanks for the reply, I will try it as soon as i get home, I am one of the furtunate ones working today, I do service and calibration of 3D measuring machines (Wenzel), bussy at BMW during their shutdown. I will let you know how i get on
Thanks Friedrich
-
Hi Friedrich,
If you're trying to use front & rear posts in the same operation, forget it. I've spent a lot of time trying to make sense of it, and the answer is that it doesn't work at the moment. The offsets work fine until you change toolposts, then everything gets messed up. I've written about it quite extensively in previous posts.
Tony
-
Hi TonyP
I only setup for front tool post, the back tool gets its offset as if it is a front tool post (or a long tool from the front) the tool is upside down so to the code it makes no diffs, if you want i will send you a pic, i use this method on my harding it works well.
thanks Friedrich
-
Ah, that's ok, so long as you don't try & change. I've managed to use tool changes & offsets with a gang tooling plate quite successfully. I use the master tool method, as described in the text. If tool 1 is the master, I would expect to see zero in it's offsets.
If you post your code I can try it on my setup.
Tony
-
Hi TonyP,
Sorry for the delay, I was working late.
Attached NC file is as posted, I tried the Tnn00 (T0200) like Graham suggested, but still no luck.
If you can test the NC file it would eliminate one factor.
I think I may have a problem in the way I am setting up the tools
I am used to using G53 for home (machine coords) and G54 for work coords
I am not sure when I setup where I am, no display of current coord.
perhaps a brief description how you setup would help. I pretty much followed the manual but may have deviated due to lack of info/understanding
Thank you
Friedrich
-
This is how i am using the coords on my Harding CNC
-
Ok, Friedrich,
I'll look at the code in the morning. I'm off to bed now!
Tony
-
Not sure about some parts of your code, e.g. G53 expects a X and Z as a distance from zero return, G28 also expects a X0 and/or Z0.
This is how I would do the code :-
Graham.
%
(PROGRAM NAME - LOCKNUT GW VERSION)
G21 G40 (units)
G28 X0 Z0 ( home Pos)
G18 (xz plane)
G61 (EXACT STOP)
G80 (Cancel canned cycles)
G95 (feed/rev)
N2 T0202 (TOOL - 2 OFFSET - 7)
(N151.2-200.5E INSERT - N151.2-200-5E)
G54 G00 G90 G43 X12.95 Z10. M8
G97 S450 M3
G1 X8.95 F.15
X-.722
Z12.
G0 X-.4
Z11.
G1 Z10.
X7.35
G3 X7.95 Z9.7 K-.3
G1 Z.4
X9.95
G0 X10.95
Z2.471
G1 X5.528
G0 X10.95
Z.6
G1 X4.82
G0 X10.95
X11.95
Z.4
G1 X7.95
X4.42
G0 X11.95
Z5.756
X10.778
G1 X7.95 Z4.342
G3 X7.698 Z4.098 I-.3
G2 X4.612 Z1.649 I2.201 K-3.098
G3 X4.42 Z1.476 I-.296 K.051
G1 Z.4
X4.62 Z.5
G0 X11.95
X50. Z50. M9
M5
M1
N19 T1919 (TOOL - 19 OFFSET - 19)
(2SD4 SLOT BORE INSERT - 2SD4 SLOT BORE)
G54 G00 G90 G43 X5.02 Z13.4 M8
G97 S450 M3
G1 Z12.4 F.05
Z6.05
Z10.05
G0 Z13.4
X5.94
G1 Z12.4
Z6.05
Z10.05
G0 Z10.707
X8.754
G1 X7.34 Z10.
X7.14
G2 X6.94 Z9.9 K-.1
G1 Z6.
X4.1
Z3.2
Z8.2
G00 X12. (ADDED THIS LINE)
Z11.
X50. Z50. M9
M5
M1
N2 T0202(TOOL - 2 OFFSET - 7)
(N151.2-200.5E INSERT - N151.2-200-5E)
G54 G00 G90 G43 X10.05 Z1.4 M8
G97 S450 M3
X8.42
G1 X-.4 F.05
G0 X8.42
X10.05
G00 X50. Z50. M9
G28 X0 Z0
M5
M30
%
-
Graham
Thank you for the code cant wait to try it tonight, my code was posted using the post for my harding, and works like that, amazing as that may seem. I will change my post to post the way you set it out for me
Thanks Friedrich :)