Internal Addressing Error

[BobL]

I recently purchased a 1993 Explorer I with a DX32 V2.30/4.54 operating system. I also purchased a OneCNC cad/cam to convert my Solid works drawings to machine code.

I can copy a .txt post from the A drive to the C drive but when I try to move it to the BMDC to run the program I get either a "Parser #4 internal addressing error "or the same thing only #10.

Can anyone tell me what these error codes mean?
Would setting up a DNC help? Or does someone know of a change I need to make to the post?

[machintek]

How big is the part program file? The BMDC has a memory capacity of 256K. If it is bigger than that, you will have to DNC.

George

[BobL]

The files have been very small 1k-2k. A simple procedure of milling .05" off of a face of a small Aluminum block.

[HuFlungDung]

Could the problem have anything to do with the start and end line characters of your program? George can perhaps fill you in on what these should be, if you are unsure.

[machintek]

It could be a bad (incorrect) post processor. Have you tried writing the program at the machine? I am of the opinion that having a CAM system does not mean it absolves you from knowing how to write a program longhand thus also knowing how to read a program to see if there are errors. I see this more and more in the field.

George

[HuFlungDung]

BobL,
If the Boss5 uses standard protocall, you need to check to see if there is a % sign at the beginning and end of your program. Now, this can be hardcoded into your OneCNC post through ncsetup, or else, you can add it in the start and end lines of the communication utility that starts from the NC editor window.

If Boss5 uses one of the unprintable ASCII characters (known as control codes) to start, then these must be entered in the start and end lines of the comm utility.

[BobL]

Hi Guys, I'm new to the machining & the cam world. So I have quite a learning curve ahead.
I've used the DX32 & the BOSS10 postprocessor with basically the same results as noted originally. I've tried modifying the post by deleting some words that didn't seem correct like an M05 that preceded a G40 G49 G80 in a Block. My owners manual says the following format must be used for the machine to work, N_G_(A,Y,Z,)F_M_(EOB). So it appears to me the G code has to be before the M code in a block. I'm suprised something so basic would be overlooked by OneCNC.

The previous owner mentioned using BOSS 10 as a post he used. He always wrote in a subroutine fashion. However being new to the cnc world I can tell imeddiately there is no way I could write the type of code needed to mill some of the parts I have designed. So I'm depending on the cam to do most of the work.

The manuals on this machine are not desinged for a complete beginner like myself, they don't say anything about a beginning or ending code format or command. None of the examples show a % sign in them anywhere.

When I first started looking for help I was directed to a gentleman that sells Camworks. I sent him a copy one one of my files and he said it was a Fanuc type post, even though in OneCNC I had selected both BOSS10 or DX32 , which by the way did start & end with a %. I even tried deleting that but still keep gettting the internal addressing error.

[HuFlungDung]

Post a small sample of a file you are trying to run. Maybe we can pare it down to the basics to find out what will work.

I'm not sure how you've got this control working with your PC, but since the controller is fairly old, make certain that your file names are legal DOS names, no longer than 8 characters, plus the extension.

[BobL]

All of my file names have been more than 8 characters, so I'll try changing the file name and run it tomorrow. Here's an example file that gets the Parser#4 error ,if I remember correctly.

[HuFlungDung]

More things to try: looking at your sample program, delete all comments, with parenthesis, as you controller may not be able to cope with comments in the program.

Round all feedrates off to one decimal place.

Place all Z movements on a seperate line (in case the control cannot do 3 axis interpolation).

Try G43 H1 on a line by itself. You don't need the D1 unless you are doing G41/G42 radius compensation. You may also have to introduce a Z movement on the line with the G43 H1.

I'm sure some guys who actually run this brand of cnc can comment on the proper syntax for you to program with.

[machintek]

Shoot! This is a machine that runs on DOS 6.20 and you have to follow DOS rules!!
You may need to get a copy of my bible: DOS FOR DUMMIES.
Your program name which is your file name cannot exceed 8 characters and it cannot contain illegal ones.

George

[BobL]

Hey guys thanks for all of your help!! Finally got my machine to make some chips. I think the parenthesis might have been a problem, but putting a colon before them did the trick. I also corrected the length of the file name & had to remove some uneeded words or even a whole block. My guess if you delete a block you can't leave the space blank, but have to delete the row as well.