[Geof]

Yes I was sloppy when I read the description for W and K; I saw the 'allowance' and skimmed over the 'rough' and 'finish'.

And I went back and looked at the paths with the two lines in and out; and I think now I understand it better

With them out the G70 starts from the same start point as the G71; X.575, Z.1. This is the spot that the tool moves to after the final run through on the G71 and after the G70 it returns here then does the G28.

With them in the G70 moves from the spot where the G71 has returned to, the original start point, up to X21. Z.1 and in doing so defines a new start point. At the end of the G70 it returns from the final path coordinate X.6 Z-2.375 in a rapid to the new start point. Because this is a rapid with by X and Z motion both axes move simultaneously until one reaches it destination then continues linear until the second gets there. So the tool does a retract at 45 degrees which takes it into the side of the hole.

[Geof]

...... It worked when I ended at X1.195, Z-1.190 but that meant I was unable to really finish the far, inside wall.....

What I wanted it to do was just end at X0.790, retract about 0.010 and rapid out of the hole.....

I started playing around and as soon as I had typed in a few coordinates a bell rang in my memory.

Here is what will not work, this must be close to what you had. Yes the problem is the move to X0.79 on line N13, this is a smaller diameter than the starting X0.875.

The reason I remember doing something similar is that the error message; 'stroke exceeds start position' totally threw me. I got hung up on stroke meaning there was something wrong with my Z coordinates and got totally puzzled.

N6 G00 X0.875 Z0.1
N7 G71 P10 Q16 D0.03 U0. W0. F0.005
N8 G00 X1.025 Z0.001
N9 G01 X0.975 Z-0.025 F0.002
N10 Z-0.22
N11 X1.195 Z-0.824
N12 Z-1.9
N13 X0.79
N14 Z-2.45
N15 G70 P10 Q16
N16 G97 G00 Z6.

[Donkey Hotey]

So to get around that problem, I could have simply changed line 6 to start at X0.5? If it's smaller than the finish bore, I'd have been okay, right? I can run this on the machine to be sure but it's tough to judge distances outside the part. And I'm a little hesitant to stick a boring bar down there to find out for sure.

I should probably cut it in air, clear of the chuck, become friends with the Single Block button and watch the coordinates.

[Geof]

So to get around that problem, I could have simply changed line 6 to start at X0.5?......

......I should probably cut it in air, clear of the chuck, become friends with the Single Block button and watch the coordinates.

Start at X0.5? No, life would be even more interesting if you did that because your boring bar would probably cram into the back of the hole. Actually you finished up doing it the just about the only way it can be done I think, in two steps. If I was doing that part I would drill a 3/4" hole and starting at X0.75 bore the .975" dia to Z-1.9 then down to X0.79 and through to the Z-2.45 usinf a 5/8" shank boring bar. Then I would use a 3/4" bar with a longish trapezoidal insert the just do the relief inside the bore starting at X0.975 and at the Z-1.9 just coming back to the X0.975

Become friends with Single Block, YES but, I think, even more important become friends with GRAPHICS. You can zoom graphics in so your tool path fills the screen, on newer machines you can slow down the graphics execution and you can have the position displayed in WORK, OPERATOR, DISTANCE TO GO or MACHINE coordinates. MACHINE coordinates are very usefule; run graphics and get the machine coordinate X for the retract move on the first cut of a G71 then Handle Jog the tool to this X position and see if the backside of the tool is going to hit the back side of the bore. "Calibrate" your tools in the sense that if you start with a 0.875" drill hole and a 3/4" boring bar you are confident that you will never get backside contact.

I have even taped bits of paper on the screen and then used the trace as a scale to draw in where the backside of the holes is along with the size of the boring bar to make sure I have clearance.

[Donkey Hotey]

How do you slow down the graphics? I know about zoom and pan but I didn't see anything about speed (other than feed hold). It's a July 2007 LCD15 so I think it's the latest software.

Yes, I had pre-bored the hole to the X0.975 diameter but I'm thinking that if the move just before doing the inside cavity had been at X0.5 before entry, it would have retracted correctly.

[Geof]

How do you slow down the graphics?......

.....Yes, I had pre-bored the hole to the X0.975 diameter but I'm thinking that if the move just before doing the inside cavity had been at X0.5 before entry, it would have retracted correctly.

Your machine must be too old to have it. I don't recall where I read it but it was three or four months ago I think that it was supposed to be coming. If you zoom in as tight as possible that slows it down a bit, And you can also single block. I know the big screen LCD does graphics in a flash using full screen.

I think you are overlooking your tool dia with the move to X0.5; you need at least a 3/4" bar in order to have the reach to do the 0.11" radial depth on the canity and I think you would find something bumping. Write the code and run through it in Graphics noting the machine coordinates then jog the machine around to see where it wants to put the bar.

[Donkey Hotey]

The bar was not the insert type. It was a 3/4" shank at the root end but it necked down quite a bit and had a 0.6" dia at the tip.

The inside cavity was designed around that bar. If it had any more overhang, the cavity would have been larger diameter (the goal was to reduce weight).

Even preboring the hole to 0.790, I would have back clearance. Retracting the 'tip' of the boring bar to 0.5 would only put the backside at -0.1, leaving 0.295 clearance.

In any case, I thank you all for this discussion. I think I understand now. The Haas manual gives decent instructions if you already understand how it works.

So now: why do I care about Type 1 and Type 2 profiles? The profile I programmed is clearly a Type 2 (X reverses on itself) but I don't see what it affected in the programming. There was no switch to tell the G71 that it was doing a Type 2 profile. It just did it. Who cares? Why do they talk about it in the manual?

[Geof]

... The Haas manual gives decent instructions if you already understand how it works.

.... There was no switch to tell the G71 that it was doing a Type 2 profile. It just did it. Who cares? Why do they talk about it in the manual?

That is so true about the manual.

There is a 'switch', I think, but refer to the manual; when the P line has a G00 for first move Type 2 is selected but if the first move is G01 or I suppose G02/3 then Type 1 is selected. I think there is some mention of this in the manual. I habitually leave the first move as a G00.

[SeymourDumore]

Geof and Donkey

If the P line is a single axis move _ G00 or G01 - then Type I is selected
If the P block is a 2 axis move, even if it's a zero move, Type II is selected.
Alternatively, if you're set to Yasnac, you may specify R1 on the G71 block to indicate Type II roughing.

Type I:

a:
G00 X2. Z.05
G71 D.1 P10 Q50 U.01 W.003 F.01
N10 G00 X.5
...

b:
G00 X2. Z.05
G71 D.1 P10 Q50 U.01 W.003 F.01
N10 G01 X.5
...


Type II:

a:
G00 X2. Z.05
G71 D.1 P10 Q50 U.01 W.003 F.01
N10 G00 X.5 Z.05
...

b:
G00 X2. Z.05
G71 D.1 P10 Q50 U.01 W.003 F.01
N10 G01 X.5 Z.05
...

In Yasnac, Type II is:

G00 X2. Z.05
G71 D.1 P10 Q50 U.01 W.003 F.01 R1
N10 G00 X.5

[Geof]

I also habitually use a two axis move so I guess I covered myself without knowing exactly what I was doing. I know I get type 2 which is what I want most times.

[Donkey Hotey]

Wow! Again: learning more than I did from hours of staring at the manual.

Last question and I think I'll finally understand this:

U and I allowances (X direction): if they're on an inside turning operation, is the allowance going to be positive or negative?

My guess is that the profile operations of G71/G72/G73 assume turning from the outside. Therefore a positive U or I would add to the dimension.

So to leave remaining material inside a bore, I would use a negative U/I (to reduce the diameter). True? Not?

The parts I made were not measureable inside. I was too busy clearing clogged chips from the bore to worry about the finish passes to notice if they were cutting material or if I had inadvertantly overcut the diameters.

[SeymourDumore]

The U W I and K is signed for the purpose of determenining the allowance amount AND direction.
IOW, yes, for OD work U and I is positive, while for ID it is typically negative.
Ditto for W and K, which also means that care must be taken when using it with cutter comp and TypeII roughing on the back side. If W-.005 is used and you're cutting the back of the part, you'll be most likely overcut the part by .005.
So, to properly state, the UWIK ( or WUKI) is actually not a true offset of the path, rather a shift in the defined direction.

[Donkey Hotey]

So, to properly state, the UWIK ( or WUKI) is actually not a true offset of the path, rather a shift in the defined direction.

Why couldn't they just word it that way in the manual? So simple. It all makes sense now. Thank you.

Yes, I kept thinking it was an offset and couldn't get my brain around all the warnings about overcut and undercut in Z.

If Oxnard were closer, I'd beg for a job in their Tech Pubs department. I think the people writing this stuff are either too close to the programming to explain it to a new user or they're so familiar with it that it makes intuitive sense to them.

[Geof]

..... I was too busy clearing clogged chips from the bore to worry about the finish passes.....

Okay now do you want to discuss how to avoid chips clogging by using G74 and G75?

[Donkey Hotey]

I'm guessing that you use G75 to peck-groove most of the material. That gives broken chips and leaves little to clean up during the G71 cycle. Am I warm?

[Geof]

Right on . When you are removing rectangular cross sections it is dead simple to program one or more G74/75 sequences to chew things off in little chips; actually it is almost essential to do it this way with 6061. I have even done it for spherical profiles where I spent a few minutes calculating the X and Z coordinates to step around the curve and then do the finishing with G71 or G72. I suppose if I wanted to get really competent I could use the G73, is it(?), the one that can be programmed to rough around a contoured path; the manual describ es it for roughing a cast contour surface I think.