Problem- G41 / G42 question

[mi2011]

Hi, I was wondering if I could get some advice in regards how G41 and G42 are used. I have the following sample code that I use on my Sherline & CNC 2.

%
G00 G90 G40 X0 Y0 Z0
G42 D1 G01 Y-40 F100
G01 Z-.2 F100
G01 X25
G01 Y0 F100
G40
G28
%

I use a 1 mm diameter end mill that is set as tool 1. If I use the code above I notice that the comp is only .5 mm. I was wondering if somebody could explain in a bit more detail what D# actually is. I was left in the impression it gets the diameter from for tool # from the tool table. Is this correct?

Am I missing anything while using G41 / G42?

I would appreciate if you could point me in the right direction. Thanks.

Regards, Michael

[HuFlungDung]

I don't know anything about your particular controls but the D number should reference a diameter value that you have entered in a register with that address. A register is just a slot in memory, a slot with an address of a D and a 1 in your example.

The other thing to understand about compensation is that it may not work correctly with a Z movement included. Convention says that the tool should be set to depth, and then radius compensation should be called. If you can get away with Z movements included, then I guess you can, but I would avoid doing that when you are just trying to understand what is going on.

Thirdly, radius compensation requires what we call a lead in to the part profile before you begin cutting, and a lead out from the part profile (when cutting is completed). This is because the control needs to see a linear movement before it can assign a left or right handedness to the next commanded movement. That is to say, offset left or offset right is ambiguous when you don't know what direction your face is pointing. So the initial lead in is equivalent to saying "Look in this direction" then the 2nd movement can be figured as right or left of the direction you are now facing.

The lead in movement should be of such a length as to equal the radius of your tool. This is to prevent an accidental gouge of the part profile that you intend to rad comp from. If the tool center is already parked on the part profile before comp is called, its pretty obvious that you've now got a semicircular gouge in the profile, that won't polish out with a bit of elbow grease

So these lead in and lead out moves have to be added as 'extra geometry' if you are working in a cad cam program to write your code. Of course, many cad cam programs make provision for adding these movements when you tell them to.

[sinha_nsit]

On Fanuc, we enter radius in D-column.

[ger21]

G41/G42 is radius compensation, so .5mm would be correct for a 1mm tool. What control are you using?

[don kruit]

G40 tool comp. off
G41 tool comp.left.
G42 tool comp.right.
G43 length of tool positive.
G44 lengt of tool negative.
D is the same as offset of you used 1.00 it is 1 mm of your work.

[Perfect Circle]

Go to this link and start at Page 247.
http://books.google.com/books?id=JNn...page&q&f=false
Good Luck~!

[rr1021ab]

if this is a mill your program is wrong give yourself more room so you can start cutter comp. if you use a .500 em your comp should be set to .250 (R)in offset page. also I did not see G56 in your program.Was the program done at the machine or on mastercam?If so Then the programer should tell you If he used it in the post .then you would set your comp to 0