[rdoty]

I've programmed a Mill Boring sub-routine (L94XX) as follows but I keep getting an "improper use of canned sub-routine" error. The format is exactly as they show it in the manual except for a "D" word. The manual says to specify an H OR D word but I can't find anything that tells me what a D word is. Anybody????

M6 T5
G0 G90 S1000 M3 X0 Y0 E3
H5 Z3. M8
G1 Z2. F8.
L9403 R0+10. R1+1.5
M5 M9
G90 G49 G0

[Wade C]

D is the diameter of the tool in the tool table.
Im pretty sure if you are in Format 2, you need to call both H and D (length and diameter) if you are in Format 1, I think that you can call the H and it will bring both length and diameter... but youll want to check that, because Im not sure, and only focused on learning Format 2.

Cheers
Wade

[DareBee]

You do not need to use D or H in format 2.
However - It is next to impossible to machine anything without using H though (height offset).
I very very rarely ever use a D.

[Wade C]

According to the manual - http://cncpros.net/Tech_files/User%2...ubroutines.pdf on page 119

They say: "1) A tool must have been specified by an H or D word and the tool diameter
MUST be in the tool table."

To me, that means in format 2, you will HAVE to have the H and the D - both called in the code, and the dia entered in the tool table.

Looking at the manual and their example, you are specifying the diameter of the bore for the L94xx cycle. So if the control doesnt know what the diameter of the tool is, how will it calculate the path? I guess, if you have D set at "0.000" that what you will get is a diameter that is what ever your R1 is PLUS the radius of the tool used.

Maybe thats the issue with the error... maybe the diameter field is blank, therefore its trying to calculate from a non-number - giving it a calculation error. If it was "0" then it might run, but give you an oversized hole?

Again, not speaking from a place of experience, just from reading the manual.

Cheers
Wade

[rdoty]

Problem solved!
(Gosh, I'd still like to meet the idiot that wrote the Fadal manual)

Although the manual states enter either "H or D" and in the entire manual there is no explanation of D I did a search last night and found a footnote that said "Input the tool diameter in the tool table before using fixed subroutines and use the D word in Format 2. Now, I had already assumed that D stood for diameter but we all know what happens when you assume. Besides, the tool diameter is already listed in the offset table so why would I have to enter it twice?

So when I change the program to H5 Z3. M8 D5 it of course works (Fadal defaults the D word to the end of the command. Go figure.)

Also, the 03 as in L9403 only stands for number of rotations at the specified diameter so it's just a compensation for tool deflection hence would probably never specify more than 02.

Thanks for your inputs. Now I can go wrestle with some other confusion...and trust me I've got a lot.:drowning:

[DareBee]

Whatever - 10+ years of running my Fadal (88HS) in format 2. With all my D settings in the table at ZERO and never using a D call.
I started using a D call only for thread milling and only in the last couple of years.
Take this info however you see fit.

[rdoty]

If you keep trying you can defeat the devious mind of Fadal.

The "D WORD" confusion is solved....at least for me.

I gave up on L94XX and decided to try L9801 and in the process was "half" successful. Okay, I was completely successful...sort of.

The D WORD does not refer to diameter but to the tool number e.g. T12, H12, D12. Took me an hour of trying everything I could think of relating to diameter. So on the same line as your H## you need to include D##. Anyway, that's what works in L9801, haven't tried it in L94XX yet.

Now, as Paul Harvey would have said, for the rest of the story.

In L9801 there are three variables...R0+, R1+ and R2+. R0+ is the feed rate (now why would they deviate from F is anybodys guess) R1+ is, get this, tool corner radius and the manual says that the larger the number can affect stepover. Ponder this while you're sitting on the stool next time. Stepover when mill boring a hole is affected by the tool corner radius?! In fact, at least in my controller, changing the value of R1+ doesn't do anything (I tried .01, .1, .5, 1.). Nada.

R2+ is the bore diameter...and believe it or not it really is!

Since I wanted a bore which would require too much stepover I took the easy way out....just used two L9801's in succession. Works for me.

Anyway, hope that clears up the mysterious D WORD as it applies to Fadals sub-routines.

[Wade C]

I guess I dont follow how it is programmed differently than 94xx - both say:

"A tool must have been specified by an H or D word and the tool diameter
MUST be in the tool table."

.... and in Format 2, Im pretty sure that you have to call both... format 1, I think it automatically takes the D from the table when you call the H (ie calling H4 - the control will take D4 from the table on its own)

Both of those fixed subroutines - the control has to know the diameter of the tool to calculate the paths and or diameter of the hole/pocket.

But, at least you got er working... and thats what matters!

Taking my info from here: http://www.fadalcnc.com/Tech_files/U...ubroutines.pdf

So I could be misinterpreting it.

Wade

[DareBee]

Ahhhhh - I see what is going on here.
Sorry for misunderstanding

I don't use fadal canned routines.
It appears that the canned routines HAVE to have a diameter call, because the are programmed to use it for size compensation (much like I use it for thread milling).

For the record, you do not need to program an H or D in a g-code file for it to run in the control.

[rdoty]

To clarify that Fadal statement....

what they are saying is that you need to specify in the tool offset table the actual diameter of the tool e.g. for T12 it's a 0.500 dia EM (or maybe 0.485 dia if it's been resharpened). It uses that value to accurately bore a hole.

Then....the so called D WORD e.g. D12 only confirms to Fadal that you really do want the T12 tool diameter. I agree it's sort of illogical but that's the way they did it.

I've got the line in my program as H17 Z1.25 M8 D17 P2000 (the P2000 is only a pause to allow the coolant to come on.

Hope that helps.

Be aware that often Fadal, and maybe others, will rearrange the order of commands, also sometimes illogically e.g. if I enter H17 D17 Z1.25 M8 it actually comes out H17 Z1.25 M8 D17. Whatever floats their boat!

I struggle with a lot of this too....sort of trying to talk like Yoda in Star Wars. It works but damn that's not the way I learned.

[DareBee]

To clarify that Fadal statement....

what they are saying is that you need to specify in the tool offset table the actual diameter of the tool e.g. for T12 it's a 0.500 dia EM (or maybe 0.485 dia if it's been resharpened). It uses that value to accurately bore a hole.

That is correct.
Then if you adjust the dia in the table (regardless of tool size) you can tweak the size of the (in this case) hole.