Offsets - How to set

[FastFieros]

I cannot get my offsets to work in my machine on the dia. of the end mills.

I have 88HS SYS95 Format 1

I am in the offsets menu and go to 2nd page is the tools. I can select the correct tool number and change the lenght no problem there. It is the diameter that will not change to something that makes a difference.

I have a part and I messed up the contour just .040 .. I just simply want to tighten up the contour around the part to erase the mistake. The end mill is .500 ... I set the offset dia. to .4400 and it still just cuts the same path as before.

The program was setup with MasterCam. I know there is a box under parameters that defines the computer, machine, no wear, ..... ( something like that anyway ) .. but I always thought that it was assumed you will be using a .500 if you tell it you are using a .500 and all measurements would be based from there. The machine would be .500 unless you had a reshapen end mill that measured .4900, and you put in .4900...

TIA..

[Neal]

If you programmed the center of the tool, then you would use only an adjustment value suchas -.003 or positive .003 which ever would be appropriate. If you programm ed the part path you would put a value over your .5 such as .504 or .497 which is appropriate.

[GM81]

I also use MasterCam, and I prefer using "wear". Then you simply leave the Diameter offset .0000 unless you need to make and adjustment. Its all a matter of preference. If you select "Computer" the diameter offset will not do anything.

[FastFieros]

Ok, going to 'wear' it adds a G41 and G40.. The G41 has D0 next to it. I am guessing that I set my dia setting in the Fadal to 0.00 now? Then if I want to comp the bit I just set it -.040 ?

[GM81]

Hmm, I don't know why it is putting out D0, the D# should match what ever tool number you have selected for the operation in MasterCam. From what you posted, you do want -.040 for your offset, but you need to change the D# to match the tool number.

Draw a line in mastercam a inch long running in X, and throw out a contour tool path using a .5 EM, and set the parameter to "computer" and post it. Then do the same and set the parameter to "wear". Look at how the post has changed. Hope this helped.

[FastFieros]

Ok .. my bad on the D0.. i set it to that in Mastercam. I thought it was D0 as in 0 offset on the .500 number ... need to read mastercam books some more.

So now i understand I will put .500 in the Dia offset in the machine tool offset screen as I have always, but when I need to comp say .040 it will be .460 .. thanks

[denmar]

TOOL TBLE": TOOL#1 .460,,,,-5.000
PROGRAM: H1D1

[FastFieros]

ok, this is driving me crazy...

I can change the value in the tool table offset for the DIA and it does not make a difference in placement or path of the tool ...

i have tried .400 and I put in .600 ... the tool stays in the same place.

The program is based on the PART Neal.

i have tried 'wear' .. it added the G41

I have always used 'computer' and there is no G41

Here is the G code. Any one see anything that is missing? it cuts the part out fine. I had a couple of these parts where the material was just a bit undersize and the part looks 'odd' .. still functions fine, but I can cut .025 off the total size no problem if I can just get the machine to work with me. I know i can go back to MasterCam and just simply reduce the part size there by thousands and generate a part path code, but this is not the first time i have wanted to comp the bit and get it to move just a little.

Some one at one time mention in a posting to someone else that the older Sys96 or maybe sys95 did not do dia comp . the value was just there as a place holder so you would know what tool you were working with. I find that hard to believe, but mine sure does not want to move that tool end mill any.

N5400 ( 1/2 FLAT ENDMILL TOOL - 3 DIA. OFF. - 3 LEN. - 3 DIA - 0.5 )
N5410T3M6
N5420G0G90S2111M3E1X2.325Y-.69
N5430H3Z5.M8
N5440Z.1
N5450G1Z-.202F6.42
N5460G41D3X-.0001F12.42
N5470G2X-.3338Y.6039I.0001J.69
N5480G1X2.8953Y2.3891
N5490G2X3.7931Y2.2002I.3428J-.5989
N5500G1X5.1919Y.4272
N5510G2X4.65Y-.69I-.5419J-.4272
N5520G1G40X2.325
N5610G0Z5.
N5620M5M9
N5630G90H0Z0.
N5640M1

[Superman]

Your main problem is how mastercam is used

tool defining should be T# = H# = D#
eg T1, H1, D1
T1 is used for the path, H1 means the program will look-up the length offset stored in the machine's tool data table, and the same goes for the D1
NOTE --- normally the D is a radius value NOT diameter ie T1=1/2" tool, then D1=0.2500 ( this depends on the compensation type used in mastercam )

Mastercam comps
Computor = No G41/42 or G40 is output, toolpath locked to tool size in mastercam ( altering comps in the machine is not effective ) ( changing tool size requires re-posting )
Control = G41/42 and G40 are output, toolpath is the contour shape ( D# is set to tool radius ) ( lead in/out must be larger than tool radius )
Wear = G41/42 & g40 are output, toolpath is offset from the selected contour ( D# is set to zero, +value = stay off the profile , -ive = cut deeper ) ( lead in/out refers to tool center-line )
Reverse Wear = not really used ( opposite to "Wear" )
Off = no comps, no lead in/out ( generally you may use for a slot type operation, or single pass with multiple depths )

[FastFieros]

I just finally went back to MasterCam and xtransform the scale .75% and that is about .040 overall ... i give up on the machine comp dia offsets. I know the lenght works 100%, the fixture offsets work, just the diameter has never worked. I have read the G codes for comp, G41 makes sense to me, but G42 does not. I can tell you that put a G42 in there and it makes the end mill take a sharp right hand turn into the part about .500 if you are paying attention. I have a nice big mistake now in that part. Glad I have 50 of these parts. Well, 49 usable ones now.