Need help to convert nc files to nci files

[AlphaD]

Can anyone help me in this problem? I need to convert .nc files into .nci files. How can I do this? Is there a program that makes this conversion?

Thank you.

[neil qwerty]

Welcome to the forum. There used to be a reverse post that you could run NC files thru to create NCI files but I haven't done that for years (before version X). It may have been a chook, I can't quite remember. What version are you using?

[AlphaD]

Thanks for quick answer. I am using Mastercam x3. I am trying to insert in my toolpaths , the code ( .nc files) , to check also some old programs .

Thank you.

[AlphaD]

I have created some programs for milling, and I have generated .nc files and .nci files. I have checked the programs by importing into the toolpaths the .nci files. I had now some other programs , but only in .nc format and if I try to import them into the toolpath , didn't get any result ( I have tried to save .nc files in .nci files , but they look the same in Mastercam editor ). I have opened my .nci files (generated with mastercam ), and the code is different.

As I am new in mastercam, I don't know how to insert these .nc files.

[Goldorak]

try to use "manual entry", then choose the .NC file to add in your program

 

this should wirk if your .nc is not too big

[AlphaD]

Thanks, but this does not work.Already tried it , but I don't get any result. As I understood, manual entry is used only for adding some text to the program. It seems strange to me that you can not write also a part of a program , manualy , as you can do it on tha CNC machine.

[mowens]

Isn't there a button you can click to choose "as code"? It's been a while so I'm going from memory here, but I'm pretty sure I used to do that.

[AlphaD]

Thanks for replies . I see that is not clear what I am asking. I have the .nc file , as text and I need to convert it into .nci file , because , I saw that with this file , I am able to create a toolpath wich I can simulate and check directly in mastercam. That's why I want to know if is possible to generate .nci files from .nc files .

[Bill Sp]

I believe the last version to do that is V7, and it was called reverse post as Neil said.

[Charlie Pierson]

V9 can reverse post

[Charlie Pierson]

They dropped reverse posting with X, methinks

[edison_tu]

V9 can reverse post,They dropped reverse posting with X, methinks----------Yes, I think so.

[AlphaD]

Thanks for replies. I will try V9 for this issue.

[Richard Thomas - Mastercam UK]

We at 4D Engineering used to sell a reverse post c-hook between V7 - V9, but it was so much trouble to maintain and update we stopped selling it (trying to reverse post/handle canned drilling cycles, tool change macros and manual edits were a couple of the problem areas).

 

V9 has a Fanuc based reverse post processor included though....

 

You need to go to NC Utils, Post Proc. You won't see Reverse as an option in V9 until you do this:

 

1) You need to edit your post TXT file. If your post is called Fred.pst (in C:mcam9millposts), you should also have a Fred.txt. If not I'm not sure that you can get this method to work.

 

2) You need to edit the start of the post TXT file to read like this:

 

menu 1 {

"Post Processor:",

"&Change",

"&Run",

"Re&verse",

"",

"",

"",

"",

"Run &old",

"",

"&Update PST"}

 

3) You will also need the actual reverse post processor called RPFAN.PST (which should already be in the posts folder) and it needs to be called by editing question #93 in you normal post processor like this:

 

93. Reverse post PST file name? RPFAN

 

4) Once the files are altered and saved, reload your normal post by going NC Utils, Post Proc, Change - just reselect the same post. You should see the "Change" option in the menu now.

 

n.b. you will be poking around inside your post files at YOUR OWN RISK!!! At the very least make backup copies of your files first.

[cobra95kev]

There is also a NC to DXF converter someone on the forum posted. It will read NC file and output a DXF file that you could load in to MCX. I don't have it on me but I do think I have it at home. I can look later if you are interested.