Is it possible to save NC files in lower case text?

[andrewgore]

Maybe I missed something, but as the title says, is it possible that when a toolpath is processed and the nc file is saved, is there any way to make it so the file name is NOT in upper_case font? Mr. Atec control doesn't like to read files in uppercase (even in the file extension....ie file.NC).

 

Any help is appreciated. I assume I just once again missed something, but i've sat there countless times going through my configurations. Maybe its a post processor thing?

 

Andrew

[Guest]

quote:

---

Maybe its a post processor thing?

---

Bingo!!!!

 

It's the only way I can thionk of to do it.

 

You have to change all output fmt to the correct lower caes

[andrewgore]

Any idea where I'd go about changing this? If its a quick "toggle", ill just do it, but if its rather involved, I dont mind calling up shopware for assistance.

 

Andrew

[Kannon]

if your using cimco as a editor..

under nc functions, just click "lower case"

and it changes it all to lower case.

hth,

[Guest]

Initial thinking is simple to do but alot to do because of the quantity

 

All of the callout like these

 

code:

---

stri        "I"

strj "J"

strk "K"

strm "M"

strn "N"

stro "O"

strp "P"

srad "R"

srminus "R-"

---

Would have to to be change, everything that cause output would have to be updated

[andrewgore]

I think you might of misunderstood where I was going with this. The text inside the NC file is just fine. The problem is the actual file name itself. The "PART.NC" aspect of the file.

 

I used to just click on the file and retype in with lower case in my windows explorer, but decided earlier to make it so it always opens NC files with Mastercams editor (can't use cimco anymore as the version that came with 9 we have still been using doesn't work with 64 bit systems).

 

Anyways, now that I made it open always with MCeditor, it took away the file extension in the windows explorer.

 

Maybe that helps describe it better?

 

Thanks for the help

 

Andrew

[Kannon]

this what your lookin for?

 

progname : 1 #Use uppercase for program name

 

instead of a 1 put in a zero

 

edit:

hang on...I dont think thats what your lookin for

[andrewgore]

Kannon,

Thanks. I tried that, but apparently it still isn't doing the trick. I did however get windows to not "recognize" a proper program to open the NC files with, so now I can go back and retype in the file with extension in lower case. Ill keep messing around with the post though. Thanks

 

Andrew

[Müřlıń®]

I have a neat little exe proggy that my dad compiled for me to do just that....it is on the FTP. It was made with VB 6.0.

 

I think it is renfiles.exe in the unspecified folder..

 

Enjoy...just drop it in your NC folder. run the exe and highlight the files you want to change to lowercase, click OK and x out.

 

 

I use it every day...

[andrewgore]

sweet. only downside is that all my files are usually 1 off kind of things. I run through all my toolpaths to ensure that they're all working properly, make adjustments if needed, and then post out all toolpaths as one large toolpath. Ill see how it works out. Thanks

 

Andrew

[mowens]

In your post, the command sextnc will set it to anything you want.

 

sextnc nc

 

Should do it.

 

I have one that has to use a .ANC extension.

sextnc ANC

That's how I do it.

[Müřlıń®]

I tried that too mowens and I could never get my post to use it properly. I have no clue what I was doing wrong.

 

I know it must me something simple...I guess I am post retarded

 

So I took the easy way out...

 

Murlin teh always more than one way...

[heeler]

Can you change the NC file extension in the Control Def, files menu. Mine is set to .NC I think you can change it to say .nc Then you would just have to change your NC program name in the toolpath menu.

 

HTH

Glenn

[Scott W]

I have a similar problem with upper case extensions on nc files. We have some old controls that only recognize lower case file names, while X2 only outputs upper case.

 

I've changed my control def. and posts to lower case extensions, but still get upper case output.

 

I found a great shareware program that will change the case on file extensions in directories and sub-directories: http://www.altarsoft.com/all_file_renamer....action=download

But I would prefer to get proper output from Mastercam.

[Günther Massimo - GMCCS]

SOLUTION:

 

code:

---

 ppost$

result=rename(spathnc$+snamenc$+sextnc$, spathnc$+lcase(snamenc$)+lcase(sextnc$))

---

[Roger Martin from CNC Software]

Günther => solution!

A very simple and automatic method of "forcing" the entire NC filename to lowercase.

[Müřlıń®]

Where in your post would you add the ppost line?

 

I have put it everywhere I can think of and I still get uppercase when the file is posted.

[Roger Martin from CNC Software]

Example of ppost$ added to the std. MPFAN.PST -->

 

code:

---

peof$            #End of file for non-zero tool           

pretract

comment$

#Remove pound character to output first tool with staged tools

#if stagetool = one, pbld, n, *first_tool, e

n$, "M30", e$

mergesub$

clearsub$

mergeaux$

clearaux$

"%", e$

 

ppost$

result=rename(spathnc$+snamenc$+sextnc$, spathnc$+lcase(snamenc$)+lcase(sextnc$))

---

[Müřlıń®]

Thanks guys, finally figured out what I was doing wrong. I am an Idiot!!!

 

I thought those indentations were just for looks.

Told yas I was post retarded.....

 

DUH!!

 

Whenever I would cut and paste stuff to my post from the forum, it would all end up on the same line....

 

Lowercase is automatic now....

 

Now I need to go back and see if I can run an EXE file with PPost...

 

I have an EXE that sections up my NC files for my little DOS control emulater on one of my machines.

[Scott W]

I've tried adding the ppost$ command, with indentations on two different posts (mpcin850 and mpselca) and it has not worked for me. Is there a certain amount of spaces for the indentation or a switch that needs to be turned on for this to work?

 

Mastercam vX2

[Roger Martin from CNC Software]

Postblock names such as ppost$ must be in the first column.

NO spaces or tabs before the ppost$.

Postlines (command lines) must be indented with at least one space. You can have more than one, it is just that one is the minimum.

[Scott W]

Is there anything else that may cause the ppost$ line not to work?

It should be a simple copy/paste, enter new line and insert indentation operation.

 

[ 06-12-2007, 10:32 AM: Message edited by: Scott W ]

[Roger Martin from CNC Software]

Note that the ppost$ postblock is special, as it is called after all the files are closed.

So why does that matter?

Example: If you put this in the ppost$ postblock ->

 

code:

---

ppost$

"I am here in ppost$ !!!", e$

---

This line of text will not appear in the NC file. The NC file has already been closed before ppost$ is called.

 

Post Class is now dismissed...

 

------

 

Scott,

 

Assuming that you have entered the ppost$ and the 'rename' command properly into your PST and it still does not work.

I'd guess that the variable "result" being used in the formula is not defined in your PST.

Simple to do, just add a declaration just before the ppost$ line, like this ->

(NO spaces in front of 'result : 0')

 

code:

---

result : 0    # Must be defined!

ppost$

result = rename(spathnc$+snamenc$+sextnc$, spathnc$+lcase(snamenc$)+lcase(sextnc$))

---

[Scott W]

Thanks Roger. Yep, that's the ticket! It works great now.