Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: KNS Supply on March 17, 2008, 01:42:34 AM
-
Using Mach 3 mill. I have a G Code program that has been written using no tools.
I need to take off .010" off the outside of the shape I'm cutting.
? What's the easiest way to do this.
Please help.
-
When you say this has been written with no tools - I take it you mean drawing tools etc.
Before I could suggest an answer ( and I am not the best man to ask, but it is an interesting question) does your G Code include any Tool information - is your tool table up to date etc. I seem to think it must be because you are asking about tool wear.
Have you already used tool width offsets etc in the code, or have you written the code allowing for this in the writing.
If you have written with tool width offsets already in, then just decrease the tool dia by 20 thou and run exactly the same program again. This would, in effect be the same as adding 20 thou wear to the tool - although I have never used tool wear - and you have the added advantage of knowing the original program worked.
-
Hi thanks for the reply.
No when I say no tools I mean no tools.
I started using Mach 3 last year to cut 3 specific parts
on a dedicated machine (lathe) so I had 2 tools set up and just wrote the program to
work. Now I converted a knee mill to cnc and I will change tools manually but I need to
learn how to set up basic tools and be able to use "wear" to change the part dimensionally
when I cut it.
Please, If you can help me with this that would be great. The manually really doesn't make
too much sense
Thanks,
Brian
also how do you write in a cutter in the code so you can just change the diameter to cut a different path?
-
I think I understand your question, so I will ramble on a bit. Pick out the bits you need.
In simple milling, you are normally cutting a shape out of a flat material. This involves using and end mill, or a slot drill or some similar tools.
Since they all go in the same chuck, then the path they cut depends on their diameter.
G Code allows you to program the cutter as though it had no diameter, and so what you see on the Mach3 tool screen is the actual program you write.
Tools you use in the mill are entered into the tool table - see Config/Tool Table - and in there, for each tool, you can enter their diameters, lengths etc etc. Wear, which you keep mentioning is also included, but I do not use it, because I measure my tools with calipers, and enter that diameter in the table. I assume the big boys buying super duper tools will have a specified diameter - and add wear in microns or thous as it happens to maintain absolute accuracy.
Tools are changed by codes M6 T** the numbers following the T is the tool number in the table. The M6 code can be programmed to do several things - nothing, move to a specific location for a manual change, or operate an automatic tool changer.
Cutting a simple outline - and allowing for the tool diameter is G41 or G42 - G41 is with the tool on the left, G42 is with the tool on the right - G40 cancels the compensation.
All you do is, at the begining of the program enter G41 - and from there until a G40 cancellation, the machine will alow for the tool width of the tool that is currently being used. It changes the compensation if a new tool is added.
I do not understand, when you say you want to use "wear" to change the part dimensionally when you cut it - how many go's are you having. In theory if your machine is set up accurately, and you draw you part accurately, then the machine will cut it accurately, without, as we used to do manually - working up to the finished diameter in little cuts.
Machines can be programmed to take roughing cuts and then change tools and take a fine finish at exactly the right diameter or whatever.
Have a look through the codes on Mach3 Mill and you will see what I mean. Have a look through Mach3 Config as well.
-
Thanks It's starting to make sense.
When I say wear, what I think I should be able to do is; if I need to cut
.002 more off a side I "in theory" should be able to go into "tool wear" and
put in -.004 and that should cut .002 more off the part.
? How would a simple code look like if I wanted to use a 3/8" endmill 1" long to cut a "2 inch circular pocket" .500" deep
(so I guess the cutter would be on the right if I was cutting cw)
I need to know this so if I want to change to a .5625 cutter I won't have to redo the whole program.
Please let me know,
Thanks,
Brian
-
Basic circle code is this :-
G00 X0 Y0 Z1. (move to centre of circle)
Z.05
G01 Z-.5 F2. (feed into job)
G41 P.375 X1. F4. (comp on P=cutter dia X= radius of hole)
G03 I-1. (cut full circle)
G00 G40 X0 (take comp off)
Z1. (rapid clear)
M30
Graham.
-
Thanks Graham
I think with all of your help I getting it to work.
Thanks again
P.S. What's the best book or cd to learn G Code
I'm not an idiot but I have been called a monkey before
Monkey proof is best.
-
Just search the web, there are lots of g-code sites.
By the way, you can not be an idiot if you chose Mach3. :)
Graham.
-
I keep getting a fault " tool radius is greater than approach line 7"
What does this mean?
-
Is the I figure in the G03 line the same as the X figure in the G41 line ? If not it should be, but minus.
G41 P.375 X1. f4.
G03 I-1.
It also uses inc IJ mode.
Graham.
-
here are the first lines of this certain program.
N5 (File Name = 123dxf on Monday, March 17, 2008)
N10 (Default Mill Post)
N15 G91.1
N20 M5 M9
N25 M6 T1(TOOL Change 3/8 ball mill)
n27 g41
N30 G43 H.025
N35 G0 Z0.0000
N40 M3
N45 X0.6014 Y0.6860
N50 Z0.1000
N55 G1 Z0.0000 F5.00
N60 Y0.7705 F20.00
N65 G2 X0.9002 Y0.6014 I-0.7767 J-1.7213
N70 G1 X0.6014 Y0.6014
etc
now the program was written for a 3/8" cutter
t1 in the table says diam 0.00
when i change that diam to .375
is when i get the error message
-
N5 (File Name = 123dxf on Monday, March 17, 2008)
N10 (Default Mill Post)
N11 G20 G40 G00 G90
N15 G91.1
N20 M5 M9
N25 M6 T1(TOOL Change 3/8 ball mill)
N30 G43
N35 G0 Z0.0000
N40 M3
N45 X0.6014 Y0.6860
N50 Z0.1000
N55 G1 Z0.0000 F5.00
N60 G41 Y0.7705 F20.00
N65 G2 X0.9002 Y0.6014 I-0.7767 J-1.7213
N70 G1 X0.6014 Y0.6014
In tool table dia for tool 1 enter difference in cutters dias e.g. .375 old cutter .250 new cutter tool dia =.125
Note what I have removed and what is added.
Graham.
-
Graham,
Why do you put the g41 code where you did?
When I copied your code and took mine out
it worked like I thought it should.
But why?
Brian
-
? also what's the easiest way to do the same exact pocket but cut ccw instead of cw?
-
You have to start the G41 on the first feed move. Rapid moves vector so the start point is wrong.
You can reverse the direction by setting the X & Y scale to -1, beware that everything will be reversed.
You can put G51 in the program to reverse sections and then G50 to revert to normal.
Man you are making my grey matter work overtime. ;D
Graham.
-
That's a good thing. It keeps you on your toes.
Thanks, Graham