[WhiteZee]

i am having a problem getting our haas vf-4 mill to read the code featurecam is putting out, this has so be a simple problem. would someone mind taking a look at this code, im getting error messages: "432 Floppy Illegal Prog Name" and "433 Floppy Empty Prog Name" i would apprciate any help, thank you.

[Geof]

In places you have lines like these:

N90 X0.5746 Z-0.0379
:~leesocket01
N100 G01 X0.225 F5.0



N155 P~leesocket01 M98
N160 G00 Z1.0
N165 X-0.5009
N170 Z0.1
N175 G01 Z-0.0379 F2.5
N180 Y-0.8191 F5.0
:~leesocket02
N190 G01 X-0.225 F5.0

Whatever a :~leesocket is I am pretty sure the controller does not like it.

[Dr Honda]

Yup... that's my guess too. You are making a call to a sub program (M98) So, the internal programs still have to follow the "Oxxxxx" format.

[WhiteZee]

ok, thanks for the help. theres no reason it should be calling for a sub-program, its only doing a pocket. guess i need to jump over to the featurecam fourm, thank you.

[CJH]

I'm not familiar with featurecam, but it looks to me as though maybe the post is putting a comment or not that may have been added into the offline programming of the part. I don't usually mess too much with subprograms but have seen this a few times with other software that I've used. It generally tends to happen if you use some type op name of other than the standard software naming of particular operation. That has led to us checking out g-code in a notepad editor before we send it over to the machine. But I could be totally wrong on this since I have no knowledge of the software you're using. Just my 2 cents.

[WhiteZee]

I'm not familiar with featurecam, but it looks to me as though maybe the post is putting a comment or not that may have been added into the offline programming of the part. I don't usually mess too much with subprograms but have seen this a few times with other software that I've used. It generally tends to happen if you use some type op name of other than the standard software naming of particular operation. That has led to us checking out g-code in a notepad editor before we send it over to the machine. But I could be totally wrong on this since I have no knowledge of the software you're using. Just my 2 cents.

thanks, ill try editing it out.

[Dr Honda]

It’s not a comment. It is trying to run a loop via a macro. The M98 is a macro call. The “P” just before is the call for the program name. And the “:” is the sub program. The ~leesocket is the name of your part, so it uses that as the name.

To fix the problem… you need to manually rename them in your program to the correct format. For example

:O00001

N115 P00001 M98

Or you need to go into the post processor, and check the box that says “Disable Macros.” It wont disable all the macros… it will just disable the internal macro calls. OR… you need to massage your post processor to get it to call the macro the correct name.

[Geof]

I.....The M98 is a macro call.....

I thought M98 is an external sub-program call, M97 is an internal sub-routine call and M65 is a macro call.

[Dr Honda]

I thought M98 is an external sub-program call, M97 is an internal sub-routine call and M65 is a macro call.

Macro... sub-program... whatever. It was making a call to some other point with a label that it didn't like.

[WhiteZee]

ok, thank you very much, ill give that a try.

[gar]

070509-1427 EST USA


There needs to be a clear definition of terms for efficient communication.

In the computer field there is a reasonably useful definition for the word MACRO. The concept of SUBROUTINES is also well defined.

In the CNC field MACRO is very poorly defined. I tried a search in Google for the group of words --- cnc code definition of macro --- and saw nothing in the first results of any value. In the CNC field I generally define the useage of MACRO(S) as being an extension of the basic G-code language and the added functions that are provided.

I do not define a subroutine of any kind as a macro. In the basic G-code language of HAAS there are two subroutine calls that do not require the option of MACROS. These are G97 and G98 as previously mentioned.

The G97 is a call to a subroutine that is contained within the current program (called a local subroutine) and is located by a line number. This subroutine looks no different than any other code in the program except it must have a unique line number at the start of the subroutine, and it has a return code at the end. I do not know what happens if you do a GOTO to this line number.

The G98 is a call to some other program that is currently in the machine memory. In this case the numeric address in the call is the number of the O-number program being called.

If you have the MACROS option, then there is an additional type of subroutine call, G65, which has the added advantage of being able to pass parameters from the calling line to the called program. But G65 only works with external subroutines.

Within the scope of CNC I would classify the following items as some of the macro functions:
#100 = #100 + 5 (count by 5)
DPRNT
SIN
ABS
G65
and lots of others.

.