starting position, compensated for the tool?

[jaras]

When creating G-code for my mill from Solidcam 2008 I always get the starting position wrong. It does not start where I put the origin when setting up the coordinate system, it kind of kompensates for the tool size, very annoying. The start will be in x0 and y0 but I have to start the mill in to the material since the origin is moved half the diameter of the tool. If I'd like to cut a square I set the edge of the tool where I want the sides to be cut, but I think the normal would be to set the center of the tool in the corner of the square. Where should I change this. I searched the GPPtool and in all options for a solution but the GPP-thing just makes me confused. It set to Fanuc now. Any help is appreciated.

[HuFlungDung]

Perhaps a little diagram of your part profile and your toolpath would help us understand your problem better.

If you were to actually draw a toolpath around a square, it would have to be offset by the radius of the tool. So if the corner of the square is at X0Y0, then the tool cannot begin there because it gouges the part. So it must be offset.

There may be several different types of operations you can create in Solidcam (I don't have the program) but you might have chosen the incorrect type of operation for your situation. For example, you might have selected some sort of 'cut chain' operation, but that is usually meant for engraving type work where you do not care that the tool is cutting on both sides of the path.

A profiling operation would be more suitable where you have to maintain a dimension on one side of the tool. For this type of operation, you need to visualize that the tool must be offset and allow for it with your fixturing.

[pinguS]

Which operation are you actually using, Face / Profile ????

Have you looked at you tool compensation in the technology tab?

[jaras]

This should explain the problem better. I created a 40x40mm box in SW and set up the coordinate system in lower left corner. A 20 mm mill to cut a profile around it, set it to the outside=right side. I run the simulation and it looks fine with origin visible in lower left corner. I created the G-code and opened it in Mach3. Here is the problem visible in the Table display. When X and Y says zero the starting position is inside the square. I expect it to be in the corner where origin is defined in SC. Now when I set up the material I have start the mill in to the part, most annoying..

Pictures are G-code, coordinate setup in SolidWorks, 2D-simulation and start screen from Mach3.

%
O5000 (F_CONTOUR_T1.TAP)
( MCV-OP ) (11-DEC-2009)
(SUBROUTINES: O2 .. O0)         
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
N1 M6 T1
(TOOL -1- MILL DIA 20.0 R0. MM )
G90 G00 G40 G54
G43 H1 D31 G0 X10. Y-11. Z30. S1000 M3
M8
(----------------------)
(F-CONTOUR-T1 - PROFILE)
(----------------------)
   X10. Y-11. Z10.
   Z2.
G1 Z-10. F33
   X40. F100
G3 X51. Y0. R11.
G1 Y40.
G3 X40. Y51. R11.
G1 X0.
G3 X-11. Y40. R11.
G1 Y0.
G3 X0. Y-11. R11.
G1 X10.
G0 Z10.
M30
%

[Brakeman Bob]

On the technology tab of the SolidCAM job, left of centre is a button called "Geometry". Click on this and a Property Manager pops up and if your profile is a closed loop, the lowermost box of the PM is a gadget for modifing the start position.

What you want has nothing to do with setting the MAC - the start postions there are for use in the post processor and are usually deployed during tool change (if used at all).

If I read you right, you want the tool to come down just off one corner, do the square and move off into space perpendicular to the first cut line. This is one of those things that SolidCAM is a little cranky with - it doesn't let you start & finish a profile at a vertice. What I do if I want to machine a square is make the profile with a gap at my chose start corner and then use the aforesaid Geometry tab to extend the start & finish.

[jaras]

I now feel a bit confused. It seems like I expected the toolpath in Mach3 to be in the origin, but of course it is on the outside of the part. Thanks for the reply. Very good to find a way to move the start-point in the chain. Thanks Brakeman Bob

[HuFlungDung]

Jaras,
You may need to study the usage of the G54 work offset to move your part origin in Mach so that your gcode program will run in the correct position in your work area. Maybe you knew that