[g-codeguy]

Incremental on a lathe? I think you have to be out of your mind.

Why? See above edit. Vast majority of the time I am working with .008R, .016R or .031R inserts. Use .005 and .01 x 45 deg. chamfers a lot. All I have to figure is the start position. Rest was memorized years ago from constant use. Bore, OD, groove on part with the same size chamfer? Type in start position, cut & paste.

[Geof]

Why? See above edit. Vast majority of the time I am working with .008R, .016R or .031R inserts. Use .005 and .01 x 45 deg. chamfers a lot. All I have to figure is the start position. Rest was memorized years ago from constant use.

Not totally serious hence the big grin. I was just seeing if I could 'out-dogmatic' Seymour.

I am not as comfortable lathe programming as I am mill programming and just find the U and W less rememberable; I tend to bang in a Z and then wonder why the tool takes off heading for the spinning chuck at high speeds.

Really it is wrong to take a solid attitude one way or the other because the whole idea is to use whatever techniques allow you to get the correct parts in the shortest time with one exception.

Never, ever use G92. on the mill; I don't even know if it is a valid lathe command.

[SeymourDumore]

Not totally serious hence the big grin. I was just seeing if I could 'out-dogmatic' Seymour.

Really it is wrong to take a solid attitude one way or the other because the whole idea is to use whatever techniques allow you to get the correct parts in the shortest time

Me? Dogmatic? :boxing:

I just figure that keeping rigidly to a technique that works every time, all the time is a best way to standardize programming.
The incremental on a lathe migght work, but no point. Use full nose comp always and program actual part always.
Ditto for milling. Full diameter comp with actual part dims.
Ditto for EDM.
I see no reason whatsoever to not utilize the control's capability.

[g-codeguy]

Not totally serious hence the big grin. I was just seeing if I could 'out-dogmatic' Seymour.

I am not as comfortable lathe programming as I am mill programming and just find the U and W less rememberable; I tend to bang in a Z and then wonder why the tool takes off heading for the spinning chuck at high speeds.

Really it is wrong to take a solid attitude one way or the other because the whole idea is to use whatever techniques allow you to get the correct parts in the shortest time with one exception.

Never, ever use G92. on the mill; I don't even know if it is a valid lathe command.

G92 on our Fagor controlled lathes is used in lieu of G50 to set max RPM. G92 on the Hardinge Fanuc controlled lathes is a canned threading cycle. An old one that I never use.

See my reply to Seymour for more of my thoughts on using incremental on lathes.

[g-codeguy]

Me? Dogmatic? :boxing:

I just figure that keeping rigidly to a technique that works every time, all the time is a best way to standardize programming.
The incremental on a lathe migght work, but no point. Use full nose comp always and program actual part always.
Ditto for milling. Full diameter comp with actual part dims.
Ditto for EDM.
I see no reason whatsoever to not utilize the control's capability.

First let me say that it is obvious to me from reading your posts and Geof's posts that you both know more about machining than I ever will.

Second a bit of background. I came from programming sheet metal. No one was using tool compensation on the lathes when I started here. So I never learned. Not sure the company would have approved of my switching programming methods. A case of keeping to the technique already in place.

Third, this is where I disagree with you. Incremental on a lathe not only works, but definitely has good points. Now I am not saying that you don't have a valid point about using the control's capability. Here is a question you probably can answer for me. I always swing a radius on chamfer corners. Can programming with tool comp accomplish this? I am not adverse to learning new things. I could be talked into trying your way. But as I said, not sure it would fly here. I got, and occasionally still get, a lot of gaff from a foreman for using macro subs when I can.

I didn't use incremental moves when I started programming. If I had to fudge in a program to hold size, I had to change 4 X-dimensions. Took me a while, but I finally figured out that if I used incremental moves after figuring the start point, then all I would have to change was one X value.

I knew nothing about macros when I started. It wasn't until someone was hired to head the lathe department that I learned to use them. I had glanced at them in the Fanuc manual, but thought they were too hard for me. Their examples aren't always the easiest to understand as far as I'm concerned. Anyway once I started using macros, incremental moves proved to be of value again.

You can see that I use macro variables on each diameter in the following example. They may not be needed, but I no longer have to stop what I am doing to go and make modifications to a program that is running. I am sure that some would say that this is a terrible practice. Letting an operator have any kind of control over a program is a no-no. Whatever. Works for me. Just like I've been told my use of M92 is a bad practice. First move in it is G0G97Z.5. I will call it up while a tool is still inside the part. Never had a crash from it yet, and never will, but some think this is very bad practice. Personally I don't see a difference between it and having to program G0G97Z.5 at the end of every operation.

N300M91 (FINISH TURN)
T0303S4000M63
X.44Z.02
G1Z0F.01
X-.035F.0035
G0X.335Z.02
G1X[.3488+#500]Z.005F.015
Z0F.002
G3U.0296X.3886Z-.0062R.021
G1U.0886Z-.0505F.003 (X.467)
X[.467+#501]Z-.5501F.004
X[.4744+#502]W-.0037F.003
G3U.0111W-.0134R.019 (X.4855)
G1X[.4855+#503]Z-1.097F.006
X.6
Z-1.106
X[.49+#503]
Z-1.0889
U-.0342Z-1.106F.002
U.0342F.006
Z-1.07
X[.4855+#503]Z-1.0814F.002
G3U-.0111Z-1.0948R.019
G1U-.0244Z-1.107
X[.5399+#504]F.0035
G3U.0254W-.0053R.018F.001
G1U.0076W-.0152
G3U.0106W-.0127R.018 (X.5835)
G1Z-1.4545F.006
U.03
G0X.91
G1Z-1.4635
X[.59+#504]
Z-1.4439
U-.0392Z-1.4635F.002
U.0392F.006
Z-1.425
X[.5835+#504]Z-1.4365F.002
G3U-.0111Z-1.4499R.019
G1U-.0292Z-1.4645
X[.8434+#505]F.0035
G3U.0329Z-1.474R.019F.003
G1U.0206Z-1.4918
G3U.0051Z-1.5013R.019 (X.902)
G1Z-1.5918
G3U-.0112W-.0134R.019F.002
G1U-.0154W-.0077
X.93F.008
M92
M1

[Geof]

g-codeguy I think you are being too complimentary putting me at the same level as Seymour in the context of CNC and the 'both know more about machining than I ever will.' is not really correct; you will probably never learn or need the knowledge I have accummulated about manual machining but you already outclass me in CNC because I do not use CAM or Macros. Also my knowledge is restricted to Haas machines, I have never run any other make of CNC.

[SeymourDumore]

G-code

First off, using Macros does have it's place and I have nothing against folks using them. I don't use them for the simple reason that if a part is unique, then there is no justification for a macro. If the part is from a family of similar parts, then I still prefer to code the part explicitly. One program belongs to one part and one part only.

About the cutter comp, there is no fudging. Never, ever. If the comp can't do it, then the cut is not possible period. And yes, I do, in fact have to radius all of my corners, including chamfers and non-tangent radius blends. Not only is it possible with comp, it is the only foolproof way to do it. If the radius is toleranced tightly, such as in O-ring grooves, it is the best way to make them correct. Moreover, if you ever turn a ball, adjusting sphericity is just plain NOT POSSIBLE without full nose comp, unless you constantly adjust in CAM and repost for variations.

Lastly, if you use incremental, you MUST poke into the code itself to adjust certain areas, such as depths and stuff. Think of a stepped part where the tool deflects by .001 on the face but does not deflect on the step's wall. If you use incremental, the stepped side will be .001 deeper than the face. Cheating (fudging) the face won't help as the step will follow. Cheating the step will do the trick, but then you're deviating from the print. OK if you are used programs that do not correspont to print dims, but I prefer to use the control's ability that allows me to always program actual part dimensions.
You're a FeatureCAM user, so I am talking about part line programming.

[Geof]

....Moreover, if you ever turn a ball, adjusting sphericity is just plain NOT POSSIBLE without full nose comp, unless you constantly adjust in CAM and repost for variations...

I will second this one, I don't use CAM so i have to use tool comp.

Doing a spherical seat at the bottom of a bore is tricky until you have figured out how your machine behaves during the setting and cancelling of tool comp.

I discovered the hard way that on my Haas TL2 G71 seems to ignore tool comp but it is instated on the final G70 pass.

[g-codeguy]

G-code

First off, using Macros does have it's place and I have nothing against folks using them. I don't use them for the simple reason that if a part is unique, then there is no justification for a macro. If the part is from a family of similar parts, then I still prefer to code the part explicitly. One program belongs to one part and one part only.

About the cutter comp, there is no fudging. Never, ever. If the comp can't do it, then the cut is not possible period. And yes, I do, in fact have to radius all of my corners, including chamfers and non-tangent radius blends. Not only is it possible with comp, it is the only foolproof way to do it. If the radius is toleranced tightly, such as in O-ring grooves, it is the best way to make them correct. Moreover, if you ever turn a ball, adjusting sphericity is just plain NOT POSSIBLE without full nose comp, unless you constantly adjust in CAM and repost for variations.

Lastly, if you use incremental, you MUST poke into the code itself to adjust certain areas, such as depths and stuff. Think of a stepped part where the tool deflects by .001 on the face but does not deflect on the step's wall. If you use incremental, the stepped side will be .001 deeper than the face. Cheating (fudging) the face won't help as the step will follow. Cheating the step will do the trick, but then you're deviating from the print. OK if you are used programs that do not correspont to print dims, but I prefer to use the control's ability that allows me to always program actual part dimensions.
You're a FeatureCAM user, so I am talking about part line programming.

First let me thank you for replying. Second I hope you did not think I was criticizing you. Third I have nothing but respect for you based on what little I know of you from reading your posts. I will continue to have it until you prove me wrong.

Minor correction of the last statement first. I use Mastercam not FeatureCAM. Not that it makes a difference to your meaning. Let me add that until a little over a year ago all my programming was done manually only using Mastercam when trig would have been necessary. I simply copied a tool path from MC, and made any needed modifications to get it looking like I wanted it to. This is faster and easier than doing the trig myself. Boss now wants all my programming done in MC...IF I HAVE THE TIME. Sometimes I don't have the time.

Regarding one part/one program, back when we had 20-21 lathes I was responsible for programming 15-16 of them (plus I helped set-up at times and occasionally ran one for a short period of time when needed). One lathe is set up with thread rolls for running families of studs ranging from 10-32 to 1/2-20 UNJF 3A. Diameters in each family are the same. With rare exceptions the only thing that changes is the dimension from the face to the first shoulder. (As far as turning goes. There are other differences such as cross holes and an internal configuration that are also controlled by macros.) Writing a master program for each family freed up some time for me to spend elsewhere. We now have 29 CNC lathes, and I am responsible for 21 of them and I still do occasional setups. We now have a couple more families of studs from different materials with different dimensions than the first ones. Master programs are a big help to me. Doubt I could keep up otherwise.

I was serious when I asked you if cutter comp could swing radii on chamfers. Was hoping you would give an example of how it is done. I tried using G41/G42 on a seat shortly after I started programming lathes. Couldn't get it to work for me, so I've never looked into using them since. (With one exception noted at the end of the thread.) I already mentioned that no one before me used them either. Programming with them has to be easier than figuring TNR yourself. AND I will look at the manuals again. Maybe I will have better luck with them now that I have another 20 some years experience under my belt. I was also serious when I said I like to learn new things. One reason I love macro programming.

So if you are using the same tool to turn 4 different diameters, and need to change the size on a couple of them, how do you do it with cutter comp without modifying the program? How do you make a taper with cutter comp if it is needed without modifying the program?

In your example of the tool flexing on the face, but not the shoulders, how do you correct this with tool comp? Doesn't a comp change follow the tool? Again, these are all serious questions which I hope you will give serious answers to. If such an incidence occurs, I do not change the value, but add a variable to control the depths. Maybe next time it wouldn't deflect, or it would deflect a slightly different amount. Maybe changing insert grade or changing to a new corner will make it come out differently. The variable allows precise control without the program deviating from the drawing dimensions.

Notice that my program is not totally incremental. In the example given incremental moves are used in conjunction with a macro to control diameters not depths. However, had I also given an example of the internal operations from one of my master programs, you would see variables used to control drill and bore depths. My original master programs for these studs used incremental from the first shoulder to the second shoulder. However a .001 deflection wouldn't have mattered as there is .005 tolerance, and some also get the second shoulder ground.

I also will use a variable with incremental moves to control the width of a groove if it is tightly toleranced. When running multiple grooves, I will use separate variables on the finish diameter of each groove. The program reflects the actual drawing dimensions, but diameters and widths can be controlled with a simple change to a macro. How would you control the diameters of each groove with tool comp?

I agree with the ball comment.

About a year ago I tried a test program using G41/G42 on a Fagor controlled gangster type lathe. It either alarmed or wouldn't work right. Or both! Course Fagors are a bit different in some aspects than Fanucs. I thought I understood how to use the 1-9 values, but maybe that was part of the problem. I also started far enough away on the first feed move for the comp to take affect without gouging the part.

As you can see, I am not afraid to show my ignorance by asking questions. Asking helps with my learning. (Provided I get answers!) I only hope that it doesn't make you feel contempt for me, and thus refuse to give answers. Or feel contempt, but give answers anyway! It's the contempt part that bothers me.

[Geof]

g-codeguy; You write too much

Actually you don't because I found interesting stuff throughout most of it. I have often questioned the utility of 'family of part' macros versus multiple programs now that oodles of machine memory is no problem but your example shows their value.

Your experience with G41/G42 seems to parallel mine to some extent and I simply chickened out except when I lterally had to use it. The tool numbers I still get stuck on occasionally but one thing I found useful was sitting down at the Haas and running Graphics with and without tool comp and using different numbers. What I did was copy the program several times, easy to do with the Haas editor, so the tool was running through the same coordinate path over and over again; in Graphics this just writes a single trace on the screen. Then I put tool comp with different tool numbers in different paths so the screen trace showed the compensated path for different tool numbers as well as the un-compensated path and I actually got to the point I almost knew what I was doing. Maybe someday I should show some pictures of the part I was developing; hollow aluminum balls 2-3/4" dia. spherical within +/-0.0005"; I gave up at that level.

Your flexing on the face I guess you correct with a macro variable; you are correct tool comp doesn't help. Being macro-incompetent I developed a work-around for a similar situation using two work zeros; the cut started in one work zero and ended in another. To compensate for the deflection the end point work zero can be offset by whatever the deflection is.

Now I should stop writing otherwise you are going to complain at me.

[g-codeguy]

g-codeguy; You write too much

Yeah, I know.

Now I should stop writing otherwise you are going to complain at me.

Never happen!

[SeymourDumore]

Gcode

Again, my non utilization of macros is a preference, not a "dogma". Your useage of it is well warranted and is likely more efficient than individual coding.

Second, the tool pushing issue is not helped by comp, but the point there was about incremental vs absolute programming and not comp vs. non-comp.

Third, the chamfer radius example:
(ROUGH/FIN OD)
(VNMG)
G50 S2400
G00 G97 T404 S600 M03
G00 X3.
G00 G42 X0.596 Z-0.3172
G96 S460 M08
G01 X0.44 Z-0.3952 F0.002
G01 X0.44 Z-0.497
G01 X0.596 Z-0.497
G01 G40 X0.596 Z0.08 F0.05
G01 G42 X0.152 Z0.08
G01 X0.152 Z0. F0.003
G01 X0.4094 Z0.
G03 X0.4207 Z-0.0023 R0.008
G01 X0.4913 Z-0.0377
G03 X0.496 Z-0.0433 R0.008
G01 X0.496 Z-0.3597
G03 X0.4913 Z-0.3653 R0.008
G01 X0.4176 Z-0.4022
G02 X0.4 Z-0.4234 R0.03
G01 X0.4 Z-0.47
G02 X0.46 Z-0.5 R0.03
G01 X0.704 Z-0.5
G03 X0.72 Z-0.508 R0.008
G01 X0.72 Z-0.65
G01 X0.75 Z-0.7
G01 G40 X0.9 Z-0.7 F0.05
G97 S400 M03

Plot it and see what it does.
Notice that it assumes a .0156 R tooltip (VNMG331). If you put in a VNMG332, the program will fail on the control, and rightly so as the radius of .0312 is too big. If you did not use full tool-R comp, the lathe would run the code nonetheless and would also blow the radiuses scrapping the part.

Fourth, diameter and taper adjustments are also not a radius comp issue. It is a control issue. The way I do it is on a Haas there is a "Taper" parameter in the offset page, and more often than not it is able to completely remove tapers, ocasionally the dia. differences are also solveable.
On the Fanuc I typically choose to explicitly code the variation, and I indicate a modified block by putting a (*****) comment at the end of each block. May not be descriptive but works quite well if you get used to it.
Having said that both Haas and Fanuc is capable of changing offsets mid-block, so when making a move on one OD, moving up on a face and then making another OD cut, the control allows the change of the tool wear and even geometry offset, so you can adjust the variation exclusively in the Offset page. In my case it isn't that big of a deal, but I do know of places where the control is set up so the operators are NOT ALLOWED to edit the program, only the wear offsets. In that case the program is written with the offset switcheroo, and the job traveler is indication what offset to change for what dimension.
Now, while on that note, if you were to use incremental programming or non-comped programs, editing a single diameter dimension WOULD NOT BE SUFFICIENT!!! as the position at the end of the block would not match the requirement to make a proper radius/fillet cut as programmed.
If however you've used absolute AND full toolR comp, the control would take care of it with with guaranteed accuracy.

Geof

You've mentioned Haas's inability to use comp during a G71 cycle.
Not True!!!
Haas can in fact use comp in a G71/71 cycle. The way I use it all the time is to activate comp BEFORE calling the cycle, and deactivate it AFTER the cycle.
Here is an example of a ball roughed on it's back side using once again a VNMG tool:
(ROUGH BACK SIDE)
G50 S1400
G00 G97 T202 S400 M03
G00 G42 X0.65 Z-0.265
G96 S200 M08
G71 D0.035 P100 Q150 U0.003 W-0.003 F0.003
N100 G01 X0.63 Z-0.265
G01 X0.63 Z-0.315
G03 X0.4455 Z-0.5377 R0.315
G01 X0.25 Z-0.6355
G01 X0.25 Z-0.8
G01 X0.6 Z-0.8
N150 G01 X0.65
M09
G00 G40 G53 X-6.5 Z-8.7

NOTICE!!!
In this example I have nothing in the back of the part, so the definition of W-.003 is perfectly OK. In other cases, such as thread-reliefs on OD threads it woudl overcit the back side by .003. That means that when you use G71 be mindful that you usually MUST NOT!! define a W value. It is unidirectional, and as such it will keep the tool and the path to the defined direction, therefore overcut the part.

[Geof]

Geof

You've mentioned Haas's inability to use comp during a G71 cycle.
Not True!!!

I wrote 'seemed to'

I did do a bit of reading and I am pretty sure it was the case a few years ago that the G41/42 within the PQ block was ignored by G71 but read by G70 and there was some comment about using U and W to leave enough for the tool comped finish. Now I think both read it in the PQ block.

Yes you can call it way ahead but then you need to take some care with approach and retract moves otherwise you get the tool doing funky sideways jumps; I didn't like that with a big boring bar in a tight hole. I chickened out and simply did the final cuts using tool comp by repeating the PQ code below the Q line.

I did sort it out the correct way for some programs making brass balls and steel housings for a locking balljoint mechanism we make but that was a few years ago and since then my poor old brain has forgotten a lot of the detail. I am not doing programming and on the lathe intensely enough, or haven't been laetely, to keep things fresh.

[SeymourDumore]

Geof

The jumping around is there ( unfortunately) but it isn't caused by the G41/42.
It happens during TypeII roughing, regardless of comp.
If you run the above code without comp, it will behave exactly the same ( except for the coords)
They may have fixed it already, my SL10 is of an '01 vintage, honestly cannot recall if the MiniLathe does the same erratic movements.
Nonetheless, does look scary but those rapids are always done in air.

[g-codeguy]

Seymour, thank you very much for the code example. I don't have any software to plot it with, nor do any of our machines have the option on the control. Doesn't matter. I can "see" it by reading your code. I do understand that a .0312R insert can't make a .03R fillet.

However your code prompts me to ask another question or two. This is the 2nd example of Haas programming that I have looked at recently. I've noticed that there is a G-code on every block, and that (with the exception of the approach) there is an X and Z code on each block even when they are the same. Is this required on a Haas? Are the zeros required?

I am a bit disappointed. You have to figure trig for the radii on the chamfers. I was hoping tool comp could magically take care of it somehow.

I've used the same tool with different offsets before, but never changed them mid-block. Always pulled tool clear then called up the other offset. This requires the setup guy to make the geometry the same for both tools. Something I am not comfortable with, but as I said I do it.

Now, while on that note, if you were to use incremental programming or non-comped programs, editing a single diameter dimension WOULD NOT BE SUFFICIENT!!! as the position at the end of the block would not match the requirement to make a proper radius/fillet cut as programmed.
If however you've used absolute AND full toolR comp, the control would take care of it with with guaranteed accuracy."

I don't understand what you are trying to tell me here. Take these 2 examples.

X.9456Z0
G3U.0268W-.0056R.019
G1U.0164W-.0082
G3U.0112W-.0134R.019

or

X.95Z0
G3U.05W-.025R.025

Changing only the X dimension will change the final OD diameter, but will not change the size or looks of the radius in the 2nd example. The 1st example would still have .003R on the corners and still be a .01 x 45 degree chamfer.

Hmmm. After reading your comments a couple more times, I think you are referring to changing the size of the radius. In which case you are absolutely correct. However.......using macros......I could change the size of the radius (and have it come out correctly) by letting the operator change one variable. No program modification needed. And I can do this with an absolute starting position and then either incremental or absolute for the ending position.

[SeymourDumore]

Huhh.. all in one breath...
Ok, No, the Haas does not need modal G-codes written on each block, neither does the unchanged coordinates. I just prefer to do them for these reasons.
The G-code signifies that it is in fact a standard motion block. Not much difference on a lathe, but drill cycles on a mill specify multiple locations by only a coordinate without a G. This convention allows a clear and immediate view of what is motion and what is canned coord.
The X and Z coords entry on each block is also used for the same reason. Typically, whenever one or the other is missing, it is so for a specific reason. For example a modified diameter value would be shown as a single X specification. Also, it is easier to read and modify the code by hand without having to look back at what is one coord or the other.
These are strictly personal preferences, not a requirement by any means.

On automatic rounding. Older Haas's were able to round 90 deg. corners only. Newer ones can do any angle, so that is definiately possible. Specify the theoretical sharp point and the R value, the control will round it off automatically.

ABout the zeros in the coordinate definitions, that is one thing I absolutely hate on Fanuc!!! No matter what you type on a Haas, they will always be formatted the same.
That is, when you type X1 or X.0001 or X0.0001, the result on your display will always be X0.0001.
Ditto for G-codes. Typing G1 will always result in G01 etc etc.
That miserable Fanuc code will look like absolute crap, as it shows whatever you've typed. It won't even interpret the typing during entry, but will error out when it attempts to run it. IOW on a Fanuc you can type .0001, and it will eat it then, but will barf on it later. The Haas will error out right there and then due to " No axis" definition.... but that is another story altogether....

[g-codeguy]

Huhh.. all in one breath...
Ok, No, the Haas does not need modal G-codes written on each block, neither does the unchanged coordinates. I just prefer to do them for these reasons.
The G-code signifies that it is in fact a standard motion block. Not much difference on a lathe, but drill cycles on a mill specify multiple locations by only a coordinate without a G. This convention allows a clear and immediate view of what is motion and what is canned coord.
The X and Z coords entry on each block is also used for the same reason. Typically, whenever one or the other is missing, it is so for a specific reason. For example a modified diameter value would be shown as a single X specification. Also, it is easier to read and modify the code by hand without having to look back at what is one coord or the other.
These are strictly personal preferences, not a requirement by any means.

I see. It's all about personal preference. To each his own.

On automatic rounding. Older Haas's were able to round 90 deg. corners only. Newer ones can do any angle, so that is definiately possible. Specify the theoretical sharp point and the R value, the control will round it off automatically.

Now this is more what I was hoping could be done on a Fanuc. Save me some programming time.

ABout the zeros in the coordinate definitions, that is one thing I absolutely hate on Fanuc!!! No matter what you type on a Haas, they will always be formatted the same.
That is, when you type X1 or X.0001 or X0.0001, the result on your display will always be X0.0001.

Again a personal preference. I would never knowingly type in X1 for X.0001, but I don't care to see the zero before the decimal point, and will go to the trouble of removing them.

Ditto for G-codes. Typing G1 will always result in G01 etc etc.
That miserable Fanuc code will look like absolute crap, as it shows whatever you've typed. It won't even interpret the typing during entry, but will error out when it attempts to run it. IOW on a Fanuc you can type .0001, and it will eat it then, but will barf on it later. The Haas will error out right there and then due to " No axis" definition.... but that is another story altogether....

If you go to CHECK while the program is running, you can see the G01 and X0.0001 on the 18T and 21iT. On the 10T it highlights the current block and 2 more. These blocks will have the Haas type display even though you only typed G1X.0001.

On which Fanuc control can you type .0001 INSERT and the control will accept it? You can't even type this in on the OT controls. The letter is always selected first. You can of course load it using DNC. Don't know about a plain .0001 as I've never to my knowledge ever had it in a block by itself. However you can misstype G01-.0001, and it will accept it. The -.0001 is attached to the G code, and of course will alarm, as it should.

On a Fagor control it probably wouldn't load. Not 100% sure about that, but if the format isn't written correctly, it normally won't load the program.

[SeymourDumore]

Oi-TC allows the editing of the individual items in a block, so there is no pre-selection of a letter.
Maybe a parameter thing, but can be done for sure on mine.

[g-codeguy]

Oi-TC allows the editing of the individual items in a block, so there is no pre-selection of a letter.
Maybe a parameter thing, but can be done for sure on mine.

What is the difference between an Oi-TC control & an O-TC? On our control it is impossible to type a decimal or number first. Whatever letter is on that soft key will be the first thing to show. Have no idea if it is a parameter change.

On our Hitachi with a Seicos control I can cursor to a single number or letter in a comment (or word address) and change, delete, add, or change and add simply by typing in whatever it is I want to & pressing ALTER or INSERT. In other words, I could cursor to the '1' type Z, press INSERT and G1-.537 would become G1Z-.537. Or I could type in X.375Z, press INSERT and in would become G1X.375Z-.537. Is this what you are referring to on an Oi-TC control? Can't be done on our OT controls.

EDIT: I lied about the Hitachi. Only the comments can be edited this way. Today was the first time in about 2 years I had to do anything on this lathe. Can only edit whole words otherwise. Blame it on my age.

[DEAN]

Geof,

Why the G90's here?:

O00000
G10 L2 G90 P1 Z0.0 (Make sure G54 is at zero)
G10 L2 G90 P2 Z-0.5 (Set G55 forward one part thickness)
G10 L2 G90 P3 Z-1.0 (Set G56 forward two part thicknesses)
G10 L2 G90 P4 Z-1.5 (Set G57 forward three part thicknesses)
G10 L2 G90 P5 Z-2.0 (Set G58 forward four part thicknesses)