Cutter comp on helix - Ultimax II - conversational

[fasto]

Hi all, I'm making some parts where I'm planning to threadmill 3/4 NPS holes. These are 3/4" pipe thread, but straight instead of tapered. Ultimax II control on my BMC-20.

So far, I've made a bunch of nicely threadmilled holes that work just great. I'm using a single flute threadmill, it cuts only one 'v' groove at a time.

What I did was to
1) Position over the center of the hole;
2) Milling: Segment 0 with no cutter comp, z start 0.050, z end -0.500
3) Segment 1: arc out from center to full depth of thread - I could probably just make a linear move into the cut.
4) Helix CCW at the thread lead and make 10 rotations (ie sweep angle = 3600).
5) at this point the threadmill is above the workpiece, so I just go to the next op.
This makes beautiful threads. I programmed my "test hole" to be at 0,0 so the calculations were very easy. Naturally the holes in my actual pieces are going to be at some other locations, so cutter comp would be nice to use. Since I did not use cutter comp, I have to do the calculations as to where the actual endpoint of the first move is to get the thread depth that I need, which I'd like to let the control do.

The reasons why I didn't use cutter comp are:
1) I don't know when the cutter comp takes effect. The threadmill has to go down the center of the hole as the clearance is very small.
Question: do we know when the cutter comp takes effect? Is it in use during segment 0, my Z plunge into the hole? Or, does it take effect during segment 1, the first move after the Z plunge?
2) Also I couldn't seem to get the graphics backplot to show the helix when cutter comp was enabled, as it just showed a straight pull out of the hole after the arc into the cut. Or, the segment 1 arc into the cut was very wrong though I don't remember how it was wrong - seems that the plot was to take the cutter the wrong way around somehow.

Of note, the move from hole center to engaged in the cut is about 0.125 or so, and the cutter diameter is 0.471. At least on Fanuc 0M machines, you need to have a linear move greater than the amount of cutter comp or it's not applied correctly. I was not able to find any info on the Ultimax implementation of cutter comp - and I don't have room for a linear move of 0.471 / 2 = 0.235 because of the size of the cutter.

And, while I was typing this, I had an idea that might make the programming easy enough to do without using cutter comp. I'll have to wait until tomorrow to see if it works.

Sorry if I'm not toally clear, I'm really tired after 10 long days in a row.

[gthlm]

Cutter comp is awkward for threadmilling on the max 2. When I do it in conversational (very rarely these days) I don't use comp either. I believe it's active immediately which makes plunging in the right place and ramping on to the cut exactly how you want a bit hit or miss. I suppose it would be ok in some cases but with an internal full form threadmill where the cutter od is only slightly smaller than the minor dia of the thread it gets very tricky very quickly.

[fasto]

Yes, cutter comp seems to be awkward to use threadmilling.
My great idea didn't work, it was to use a Milling block with no cutter comp for the Z plunge then a new Milling block with cutter comp for the helix.

Anyway I'll just do it the hard way, although it's not really that hard.

I'm not capable of writing gcode by hand - and I don't trust my CAM program yet.

Pics when it's complete, if interested?

[pgf545]

I don't use cutter comp for thread milling either. I am a little confused by the reasoning you need to use it? When I have multiple holes to program I will program the first one at 0,0 and then use a pattern location block to position the holes. Is that what you are looking for or am I miss reading your post? Yeah post pictures when you are finished.

Bernie

[fasto]

I had hoped to use cutter comp to only have to program the x,y of the center of the hole, and the depth to which I want to threadmill. I also would compensate for possible different OD's of the threadmill.

Does a pattern location allow you to not do the original pattern? If so then I'd be able to program the pattern at 0,0 and repeat the pattern at the locations I need it - which won't be 0,0 on my part. Since my part is round, I'm using the center as 0,0 - which makes my desired locations something like -0.745, 1.020 and 0.745, 1.020 (easier for my to think in quadrants for round parts).

Just spent the last little while making soft jaw blanks so that I can hold this part: plan is to use a three-jaw chuck clamped to the table. Should work OK, once I get the right screws for the chuck jaws.

[pgf545]

You can use pattern location anyway you want. It does not need to use the location of the first hole. You could program the first hole at the -.745, 1.020 and then pattern locate the second hole at .756, 1.020 if you want or you could program at 0,0 and locate to -.745, 1.020 and .745, 1.020. I use a 3 jaw chuck sometimes but I will just use toe clamps to hold it down as long as they are not in the way of the part.

Bernie