cycles initial plane/retract plane

[HuFlungDung]

I'm just wondering whether the general consensus on how Xp's initial plane and retract plane works for machine cycles is correct for your machine?

I make it work by forcing values into the cycle wizard that do not exactly match anything in the real world. What I see in the output code is that the initial plane is being subtracted from the clearance plane as though it were an incremental value, whereas I actually need them both to be absolute values.

Does it seem to be right from where you are working from?

Example: Initial plane input 0.4
Retract plane 0.2

Output in code is:
Retract plane is at Z.2 absolute, but initial plane is Z0.2 absolute.

[wms]

Hu,
You've been messing around again, Haven't you?
The Haas post works ok.

Example: Initial plane input 0.4
Retract plane 0.2

Output in code is:
Retract plane is at Z.2 absolute, initial plane is Z0.4 absolute.

Sorry, looks like you get the short end of the stick again.:frown:

[HuFlungDung]

Here's what you use, is this correct?

{_MODE} G81 {Z} R{CT} {F}

Here is what I use:

Z{CD} /R{CT} /T{_DWELL} G81
/Z{CP}

This is because I need to see the move to the initial plane immediately after the cycle is called, to begin the autocycle.

I just think it is weird that some math operation is carried out on {CP}

[HuFlungDung]

I think it is me all right

I'm going to redo my setup of the drill cycles. I think maybe I should create a new parameter for my surface height, rather than trying to pull it out of those other variables.

The other thing I overlooked, is that the Z rapid height has to be higher than the retract height, or I'll get that "capping" effect.

[wms]

Hu,
What you have listed is correct. It is the standard haas post cfg.
But I think your problem comes in when you get to the "cycles" box. Let me try to explain.

If you look at use the Haas post, (note you have to select the post, ie haas or shadow, before you use the machine cycles) and select your points then the tool, then clearance, you will get to the cycles box. This is where there is a difference between the two.

The Haas cycles box has only: "retract mode" to check.

The shadow cycles(the one you sent me) has:
Peck dist/z
Dwell /t
Safety......../z (wouldn't this be the Retract plane?)

I tried your shadow post and I get the same results you do.

I think this extra info from the cycles box is what is causing the Heartburn. But that is only a guess. I have messed around with different values in both of the boxes , but I am not able to make things work the way you would like.

[wms]

Hu,
I miss spoke in the above post. The extra boxes are under the G83 cycle not the G81. Shame on me.

[HuFlungDung]

Thanks WMS for your input.

I fooled around with it for a while longer, and the only thing I could do was create a new parameter to hold what I would call the initial Z start, which should logically be the same as the Drill-initial plane but for whatever reason, that variable does not contain the fixed amount as taken from the user input.

It is no problem to do it this way, I just get another variable to define later in the cycle's "extras" field.

I only got to messing with this today because I was drilling some holes that started on a surface well below my Z0, and the negative numbers involved were driving my drill cycles wacky.
But anyway, now I have the post set up better than before, so that is a good thing.

I've also changed my habits with regards to the initial Rapid plane and tool offset. I developed perhaps an erronous habit of running my Z home at Z0.1 , my tool length offsets all the way down to Z0.1 and Rapiding around at Z.1 (My one mill has fairly limited 4.5 inch Z axis travel).

Instead, now I define a Z home of Z1.0, define the length offsets relative to Z1. and Rapid around at Z1. This allows me to call the tool length offset without worrying about the tool being so near the surface, and allows a little more leeway for error, should an offset happen to be slightly incorrect when it is called (the tool moves when the offset is read). This change allows me to make better use of the intermediate positions that Onecnc allows for in positioning the tool before the plunge, etc.

Say, we were agreeable on the potential benefits of a"peck-plunge" option when using end mills, what do you think about the option for Rapid plunge, as well?

I find there are times when I do start a multi-pass roughing cycle with the tool "out in the air", and this gets fairly tedious to watch the thing plunging at a typical feedrate. In the meantime, when I foresee such circumstances, I am happy enough to insert a very high plunge feedrate to accomplish the same thing as rapid, but it doesn't seem to me to be as clear to the operator as a Rapid command would, when he's checking through the code on the machine display.

[HuFlungDung]

Originally posted by wms
Hu,
I miss spoke in the above post. The extra boxes are under the G83 cycle not the G81. Shame on me.

You do realize that these extra boxes appear when you create a new parameter, right? Just testing your knowledge, this was not immediately apparent to me, either.

[wms]

Hu,
I just use the Haas post and don't need to create any new parameters.....Yet.
So I kind of knew that "STUFF" would show up in the boxes after you create new parameters. Mostly after "looking" at your shadow cfg.
I feel for you because you have to make up your own posts.
I'm spoiled in that the standard posts, so far, do every thing I need them to. Maybe I'll get creative like you and add some extra features.

Pretty neat that you can modify your post so easy in OneCNC, don't ya think?


And as far as the Rapid Plunge thing, I'm all for more features. Any thing to make my life easier.

Oh by the way... Stop testing Me....

[HuFlungDung]

Originally posted by wms
snip
Pretty neat that you can modify your post so easy in OneCNC, don't ya think?

Absolutely! I spent hundreds of hours learning about and making scripts in Bobcad to do what Onecnc can do "out of the box".

[HuFlungDung]

I suppose there is not enough user base here to get a decent poll result, but I would still like to know if the cycle "initial plane" and "retract plane" is perfect as set up.

I can see the need for a couple of different options, depending on what your controller expects. The options I am referring to are simply this: should these two planes be absolute values or incremental? Should the values be operated on mathematically or just "left alone" so to speak.

I do have sort of a system to make the resultant output come out right.

Here is what I have figured so far. Here is what I have set up in my deep hole peck cycle:

/Z{CD} Z{_PECK} /Z{_RETURNSTOP} /R{CP} /T{_DWELL} G83
/Z{_P8}

Here is how I might want a sample of code to look, where the initial plane is equal to the Rapid plane:

T4 ( 3/32 DRILL)
F12.5
S70 M3
T400
M8
/X2.6734 /Y-13.1875 /Z1. (Rapid plane absolute)
(if initial plane <> rapid plane then a value appears here)
/Z-1.2 Z-0.4 /Z-0.01 /R0.2 /T0. G83
/Z0.2 (this is the move to the initial plane, absolute in value, the cycle begins to execute at Z0.2)
/X3.1855
/X3.6976

In the above sequence the tool rapids from Z1 to Z.2, then rapids from Z.2 by the incremental distance indicated by the /R value, which brings the tool tip right to Z0. Then the drill drills an incremental Z-1.2, with a peck distance of -.4.

A chipbreak move is indicated by the /Z-0.01, which I created the variable {_RETURNSTOP} to hold. This is fine.

If the initial plane is equal to the Rapid plane, then no nc output results between the initial Rapid height and the calling of the cycle. This is okay by me.

Whatever I put into the Retract plane field is apparently subtracted from the initial plane to equal the net retract height that is output. This seems weird to me. I'd just as soon be able to type in what I want it to be in absolute, and have that exact same figure come out in my code.

For my controller, the R value is an incremental distance, that the tool will traverse (at rapid) at the start of every hole in the cycle. The end of every single cycle results in a retraction back up to where the tool started the cycle at.

Suppose Rapid height is 1", initial plane is .2" absolute and retract plane is .2" absolute. In order to make the right code, I have to enter values in the initial and retract fields that give a subtrahend of 0.2 . Thus, I would put in .2 in the initial field and 0 in the retract field. This results in nc output of .2 for the value /R{CP}. note the retract plane value of 0 is meaningless so far as where I intend to begin the tool at, which would have to be at a value of R.2

Because some kind of subtraction also seems to be performed on the initial plane variable {CP}, I cannot use it either, so instead I created this new parameter /Z{_P8}.

This is not whining. I am just wondering if there needs to be more of a "setup" to the nature of these Initial plane and Retract plane variables, depending on what various controllers require.

Perhaps it is all in the method I am thinking in, but it seems to me that the rest of the toolpath wizards operate on the principle that the various tool planes are absolute Z values, but when we get into the cycles, then all of a sudden, they switch to relative values.

I am sorry if I am not making this perfectly clear. But, you would know by now perhaps if you had any difficulty making the right input when you fill in the fields in the cycle wizard, using your own machine's cycles.

Just to test your own cycle setup, does what you have also work if you want to drill a hole at a lower level, like Z-1. down to Z-2., but maintaining your retract height at Z.2 between holes?

Maybe they should add the words "relative or incremental distance" to the Initial and Rapid planes in the cycles?

Opinions? Discussion?

[wms]

HU,

Here is a sample post. This is with the Haas cfg. Xpert program.
At the bottom is a screen shot of the setup box.
Seems to work just like it should. Sorry.:P
All figures are absolute. No addition or subtaction was done by the program.

%
O0000 (PART - )
(POSTED - FRIDAY, MAY 30, 2003 (19:03))
T1M06 (1.0 INCH HSS 1.0 DRILL)
G90 G80 G40 G55
S1505 M03
G00 X0. Y-0.6172 / M8 ( move to position)
G43 Z1. H1 (call tool height offset, also rapid plane)
Z0.2 (move to initial plane)
G81 Z-2. R-1. F5.7189 (drill cycle -1. is retract plane)
Y-3.3828
X-4.
Y-0.6172
G80
G00 Z1. (back to rapid plane)
M01
M30
%