[rckdef]

What i got is .065 Aluminum. I have a profile and two .250 holes.
I have no problem with th profile its how to do the holes
I am useing a .250 end mill. What i would like to do is cut the
profile and then plunge or drill the holes useing the same .250
end mill. I did it sucessfuly using the drill-hole dialog and chose a .250
drill to fool it. It worked! The only thing is the G-code came out with
two drilling sequences. The first sequence was correct just what i wanted
the second sequence i dont know where it came from it drilled down deeper.
me thinks maybe the center drill in the dialog has something to do with it
even though i did not choose the center drill. Must be an easier way!!
got any ideas----

[GeorgeRace]

Might it be possible that when you did the drawing you ended up with two .25 inch holes, one below the other, so you don't see it on the drawing?

George

[rckdef]

Thanks George
NO George that is not it. I re checked the drawing. I am using BC v23
The drawing i made in Solidworks, DXF it and opened it up in BC
No Problems--The G-code starts out with "Job 1 Contour" It cuts the
Profile just fine then it says "Job 2 Hole Random Point Pattern" and the
sequence goes down to G1 Z-0.08 just like i want it to.When thats done
again it says "Job 2 Hole Random Point pattern" and the sequence takes it down to G1 Z-0.1951 (where did that come from?) I dont need that second
part, of course i could delete it but i dont understand it! Do you think its
possible to plunge a hole useing an end mill in BC. I can write the G-code
to do it in my other programm, but i need it in BC.
You think im beating a dead horse?
Thanks

[SBC Cycle]

When you select a drill feature, BobCAD will automatically insert a center drill. If you want to change that for this part only, you must change the "tool pattern" for the drill feature.

In the CAM tree manager, right click Milling Tools, go down to Part, then choose Tool Pattern. In the dialog, click on HOLE and remove the center drill tool. Now when you create a drill feature, it will not call a center drill. I think this may be what you are looking for.

[SBC Cycle]

Forgot to mention, if it seems like it's going too deep, remember that BobCAD will look to see how much angle is on the point of the drill. Since you are using and (flat) end mill you don't need to go as deep. You can sort of override this by giving your "drill" a nearly flat angle, like 179 degrees or something. Hope that helps.

[jay_dizzle]

another thing you could check is in "milling tools" right click then go in to "current settings" check to see that the "output subprograms" box is not checked. this is a commom occurance at our shop. seems to come and go as it pleases.

[rckdef]

Thanks SBC
Sound like a solution ill try it
rckdef

[rckdef]

Thanks again SBC
It worked like you said----Great
rckdef

[SBC Cycle]

Sweet, glad to help