Questions on BobCad Posting & cicular Interpolation

[Malish]

We just upgraded to V22 from an older version and I have a few questions on the out put. We have a Haas TM2 and a couple of Techno routers that we program for. One of the things I have to program for the routers is to cut a center hole out of a block plastic. So when I do this in V22 I get the following code.

%
O100 (BOBCAD1.NC)
N01 (TUE. 02/19/2008 09:39AM)
N02 ( TECHNO )
N03 ( T1 ENDMILL ROUGH , Diameter = .3125 , Length = 5.)
N04 G17 G20 G49 G54 G80 G90
N05 (JOB 1 CONTOUR)
N06 (TOOL #1 0.3125 ENDMILL ROUGH)
N07 T1 M06
N08 S5000 M03
N09 G00 X-2.8438 Y0.
N10 G43 H1 Z.1
N11 M08
N12 G01 X0. Z-.375 F40.
N13 M98 P10 ( SUBPROGRAM CALL )
N14 G00 X0. Z.1
N15 M09
N16 M05
N17 M30
%

O10 (SUBPROGRAM OF O100)
G03 X-2.8438 Y0. I2.8438 J0. F60.
G01 X0. Z-.75 F40.
G03 X-2.8438 Y0. I0. J0. F60.
G01 X0. Z-1.125 F40.
G03 X-2.8438 Y0. I0. J0. F60.
M99 ( SUBPROGRAM RETURN )

Now first thing I don't like is that it does a sub prgram for the cut. Is there a way to get it to not use the sub program when posting and just put the code for the cut in the main program?

Also, we generally use a G02 instead of the G03 when cutting circles in plastic so we can go clockwise and pull the cutter into the material. Is there a way to get it to go the oppsite direction?

So basically when I cut the 6" diameter hole I would like to se the following from the post

%
O100 (BOBCAD1.NC)
N01 (TUE. 02/19/2008 09:39AM)
N02 ( TECHNO )
N03 ( T1 ENDMILL ROUGH , Diameter = .3125 , Length = 5.)
N04 G17 G20 G49 G54 G80 G90
N05 (JOB 1 CONTOUR)
N06 (TOOL #1 0.3125 ENDMILL ROUGH)
N07 T1 M06
N08 S5000 M03
N09 G00 X-2.8438 Y0.
N10 G43 H1 Z.1
N11 M08
N12 G01 X0. Z-.375 F40.
G02 X-2.8438 Y0. I2.8438 J0. F60.
G01 X0. Z-.75 F40.
G02 X-2.8438 Y0. I0. J0. F60.
G01 X0. Z-1.125 F40.
G02 X-2.8438 Y0. I0. J0. F60.
N14 G00 X0. Z.1
N15 M09
N16 M05
N17 M30
%

Anyone know how to get it to do this? Thanks

[tjones]

Sub output is on by default when installing so that is the first thing to change.

Right click the "Milling Tools" in the Cam tree. Select the "Milling Settings" under the Postings menu you need to uncheck the Output Subprograms.

You should change the direction of the contour to reverse your cutting direction. Look in the help menu for a detailed description.

[Malish]

I unchecked the output subprograms and that took care of my sub program problem.

However I can't seem to get the reverse contour to work on a circle. I even split the circle into 2 halves and it still did not work. It seems to not want to let me select it after I pick the button off the menu.

[The One]

Likely because the arc is not a contour.

Click on Other => Contour.
Select the Circle, then right click and left click OK in the pop-up menu.
Now the circle will have an arrow which depicts directionality. If the arrow is in the wrong direction, you would now use the Reverse Contour option.

Regards

[Malish]

Thanks! That seemed to take care of it.

I assume that I want to make a contour from my geometry everytime I want to make a toolpath from it? This will combine a set of arc and lines into a single profile to follow?

[The One]

As a "rule", no you do not have to use the Contour creation function. It is suggested however, so that you can control the direction of the cutter around wireframe geometry.

Yes, it does combine all of the selected entities, in a contiguous chain, into make one selectable entity, which then allows the user more control over the direction of the cut.

Regards