[mbam]

I have a simple boring operation that has a couple of small chamfers, Instead of outputting the chamfers Bobcad is outputting radius's in the code. And my lathe (Fanuc control) is ignoring that part of the program. No error's, just ignores that area of the part.


Any ideas?

[fidia]

Can you post the suspect code and image of the toolpath

[mbam]

The code and .bbcd are in the zip file (fisrt post)

My lathe just ignores the moves at the top

[SBC Cycle]

Hey Marc, I took a look and I think I see what is going on. When System Compensation is on the toolpath is going to "roll" over at all the hard edges of two intersecting lines, including chamfers. You can see that in the closeup above in your screenshots when it encounters the second chamfer. This is the first time I've looked at a BobCAD lathe file so I hope someone corrects me if I'm wrong but that's what I see as I played with the allowances and the tool nose radius.

Attachment 252176

When BobCAD offsets the toolpath for your tool allowance and trims it to the Z value (4.99) of the selected geometry, the length of the chamfer ends up measuring only 0.005" long. You can also see (in the pictures below) that when the System Compensation is applied (using the tool nose radius) and it rolls over that first edge, the difference between the path I drew manually and the toolpath BobCAD comes up with is close enough that the first line is eliminated and becomes one single arc - the rollover. This is happening because of the general allowance allowed by the system and the calculations doing the offsetting. If you could measure the variation between the two, it's probably less than that tolerance.

Attachment 252178

If I don't change anything else in your file and go to Preferences - Settings Part - System and change the Lathe tolerance to 0.0003" I manage to get a linear move at the very beginning of the bore. A lot closer to what I think the path should be but I would instead simply extend the chamfer out into air by drawing a line at an angle (Line - Angle - Relative to Entity) of 0° at least the length of your tool nose radius. That will force a linear move at the beginning, long enough to not get "toleranced" out by the System Settings and nothing else in your code should change.

[The Engine Guy]

Marc

SBC is correct, BC doesn`t work right on System Compensation, I always turn it off when using Fanuc (0T in my case) controls, if you turn off the System Comp in BC and use your tool offsets and TNR in your Fanuc control you shouldn`t have any issues

See image for toolpath without System Comp


Regards
Rob
:rainfro: :rainfro: :rainfro:

[mbam]

Thanks SBC & Rob,

I'm just getting up to speed on the lathe, so taking little baby steps

I will give that a try later. I did find my biggest problem was I had the Z tool offsets fubar so the boring bar was cutting air. Got that handled so back at it.

[WILDMAN2]

Marc

SBC is correct, BC doesn`t work right on System Compensation, I always turn it off when using Fanuc (0T in my case) controls, if you turn off the System Comp in BC and use your tool offsets and TNR in your Fanuc control you shouldn`t have any issues

See image for toolpath without System Comp


Regards
Rob
:rainfro: :rainfro: :rainfro:

I do the same turn off system comp and machine comp