Hi,

I am new to machining, albeit not CNC controlled machines. I have a 2001 vf-oe we purchased and mastercam x3. I am having trouble with the tool length offsets.

The g54 seems to work correct for x and y, but z axis doesn't seem to be pulling information from the tool definition or maybe I am just not using it right.

Does anyone have post that they use with Mastercam and a vf-oe or similar that does work for tool offsets and any pointers on what toggles to flip in Mastercam to make sure it comes out correct?

Thanks!

jack

Could you show us a line of info?
Dose it contain a G43 (height offset read)?
Jim

Yeah. I am setting the part offset via the machine and the program is calling the G43. I am using a pointer in one of the tool holders to find my zero index point and then I have put offsets in the registers for the 4 or 5 tools I use. I think I put them in relative to the length of the pointer used to find the zero point. (i.e. it is 2" long and the tool is say 2.5" so the offset is .5")

The Length for the tool offset is set in say Register2 for Tool 2 (keeping it simple). So I though the G43 H2 ZX.XX should move to the specific Z compensating for the offset.

It just seems like the X and Y are working for the part offset, but the Z isn't...even though I am setting it.

Thanks for the help!

>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>

O0000(PROGRAM NAME - 30BACK)
(DATE=DD-MM-YY - 29-12-08 TIME=HH:MM - 02:25)
(MATERIAL - STEEL INCH - 1010 - 200 BHN)
( T2 | 1 INCH FLAT ENDMILL | H2 | XY STOCK TO LEAVE - .1 | Z STOCK TO LEAVE - 0. )
( T3 | 1/2 FLAT ENDMILL | H3 | XY STOCK TO LEAVE - .05 | Z STOCK TO LEAVE - 0. )
( T4 | 1/4 BALL ENDMILL | H4 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1 INCH FLAT ENDMILL | TOOL - 2 | DIA. OFF. - 2 | LEN. - 2 | TOOL DIA. - 1. )
N104 T2 M6
N106 G0 G90 G54 X.4718 Y1.0007 S534 M3
N108 G43 H2 Z1.09
N110 G1 Z.09 F6.42
N112 X.4463 Y1.0127
N114 X.4352 Y1.0175
N116 X.3891 Y1.038

O0000(PROGRAM NAME - 30BACK)
(DATE=DD-MM-YY - 29-12-08 TIME=HH:MM - 02:25)
(MATERIAL - STEEL INCH - 1010 - 200 BHN)
( T2 | 1 INCH FLAT ENDMILL | H2 | XY STOCK TO LEAVE - .1 | Z STOCK TO LEAVE - 0. )
( T3 | 1/2 FLAT ENDMILL | H3 | XY STOCK TO LEAVE - .05 | Z STOCK TO LEAVE - 0. )
( T4 | 1/4 BALL ENDMILL | H4 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1 INCH FLAT ENDMILL | TOOL - 2 | DIA. OFF. - 2 | LEN. - 2 | TOOL DIA. - 1. )
N104 T2 M6
N106 G0 G90 G54 X.4718 Y1.0007 Z height of part S534 M3
N108 G43 H2 Z1.09
N110 G1 Z.09 F6.42
N112 X.4463 Y1.0127
N114 X.4352 Y1.0175
N116 X.3891 Y1.038

In this case Z (top of part) offset would be Zero.
You would need to rapid above the part
G00 X0 Y0 Z0
G43 H2 Z1.09
G00 Z.100
G01 Z-.09 F6.42
N112 X.4463 Y1.0127
N114 X.4352 Y1.0175
N116 X.3891 Y1.038

This would rapid above the part .100,
Feed to .09 below the surface,
Then mill in X and Y

G54 sets the offsets for all three axis,
G43 is the tool height compensation offset.

The machine needs to know where the top of the part is...G54

Yes. I know it need to know the top of the part to start. I think it isn't the machine that is the issue. MasterCAM is putting out some files where it seems it starts at Zero for the z value and other where it is adding in the thickness of the stock as the starting point.

So, on the file I just milled it worked correctly and my starting Z point was .01 or something like that where I was leaving a little stock on the cut surface in roughing. The thickness of the part/cut was about .27 for this one.

But, the file I am fighting now always seems to have a starting cut Z of 6.46 which is the thickness or height of the part.

I have tried changing the origin Z position in MasterCAM and re-posting...no effect. Thoughts?

scott

OK. I am pretty sure this is a MasterCAM issue now. I draw my parts in Solidworks. Which will have an "origin" somewhere in the drawing depending on where I start and how I "expand" it.

When I pull the drawing into MasterCAM, it is always offseting my first Z value to the origin offset from the Solidworks drawing.

What I need to do it set the origin in MasterCAM to the uppermost cut face in the drawing.

Does anyone know how to do that? Something to do with CPlane, TPlane, WCS and Gview I think....

scott

Hello

I once taught Mastercam and the golden rule was to set Z0 above the work piece. Take a side or front view. Using Analyse pick the part with the 'highest' Z value. Then use Translate, All, Entities to move everything below Z0.

This assumes that menu cammands have not changed since my day!

Good Luck

Richard

Richard,

Thanks for the reply, but those commands aren't in X3 and I haven't used a previous version to be able to figure out what they might be.

Any other thoughts?

scott

Hi Scott

The commands I quoted just allowed you to 'see' the part side on, measure the high point, and move everything, so that no point remains above Z0. This ability must be there somewhere ....... auto work has one reference on the the front bumper (fender) and you get the job for a mould of a rear light cluster ...... all references are 'miles' away!

I' m off to my bed! Good Luck!

Richard

OK. I am pretty sure this is a MasterCAM issue now. I draw my parts in Solidworks. Which will have an "origin" somewhere in the drawing depending on where I start and how I "expand" it.

When I pull the drawing into MasterCAM, it is always offseting my first Z value to the origin offset from the Solidworks drawing.

What I need to do it set the origin in MasterCAM to the uppermost cut face in the drawing.

Does anyone know how to do that? Something to do with CPlane, TPlane, WCS and Gview I think....

scott

It's in there. Xform, translate, all entities then hit enter. Translate box will appear. Several ways to translate, use the from/to area and pick the +1 button. This will let you tell mastercam you want to move your part from your zero of choice(corner, centerline, etc.) to mastercam's origin.

Yes. I found it. Move the part X, Y or Z as necessary, reset my stock and regen the cut paths.

Cutting like crazy now!

Thanks all for your input.

You can also create a new coordinate system in solidworks exactly where you want your part origin to be. Then when you import, the part will automatically be where you want it.

.

With Mastercam you can make as many view/tool planes as required. What ever you create in Solid works, should not matter to Mastercam. You as the programmer must decide where the face origin will be on the part, if not defined from the part print. Is the part complicated, surfacing, and draft cuts? or is it just a simple part with pockets, holes, ect? If it is simple, why draw it solid works, Mcam is much easier to draw with, and you do not have to worry about importing models, or rev changes.
Tool length offsets, is the setting on the Haas control set to "length uses work", on or off? This will change your measured length offsets. I am not sure what setting number it is but look in the setting page and you will see what I am talking about.