Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: wade16 on October 26, 2013, 09:31:09 PM
-
Hi,
I have an old version of EzCam 6.1 Cad program that I use to draw geometry, plot cutter paths and post the program with Boss6I post processor to get a G code file. When I load it in Mach3, the program has problems with radius generation and makes G3 CCW moves when it should be a G2 CW move. Does anyone know how to fix the differences so Boss6I will generate a usable G code to run with Mach3? I am not able to load Mach3 post processor into Ezcam, as it is in the wrong format for Ezcam. Is there any version of Mach3 post that would load into Ezcam 6.1?
-
I had some success with the arc problem by going into Mach3 and changing from INC to ABS. That seemed to fix the wandering arcs problem. I have 2 post processor files, Boss6I.cnc and Boss6I.cnx. How do I edit the post processor file to make changes? I can view the .cnx file in Word Pad and it is all normal text. The .cnc file has some text, but mostly different symbols that I can't read. Which file do I need to make the changes to?
-
Is that not a question you should be asking EZCAM ??
Just a thought, (;-) TP
-
They do not support that version anymore. I am hoping to get some help from forum members that know how to edit this post processor. I think Mach3 users will have a better idea of what changes will be required to allow the Boss6I to make a correct G code for Mach3.
-
Upload the post here and lets see what it looks like.
(;-) TP
-
I tried, but the file extension .cnc and .cnx types are not allowed to be attatched. Is there a way to attatch them in another way?
-
change the extension to TXT or zip them up and send.
(;-) TP
-
Here they are. The first one with the extension of .cnc I will name Boss.doc and the second .cnx file will be Boss.dxf
-
Are you sure this is a Ezcam Post ? It looks like an early Vectric post . Normaly the company puts there company name into the post this one has Vectric in it.
What ever it is for it is correct as far as G2/G3 are concerned. G2 is CW and G3 is CCW.
(;-) TP
-
This is a post I used on a Bridgeport CNC mill several years ago. I know the radius problem was due to a setting in Mach3. Once I changed from INC to ABS, the problem went away. I want to know how to edit the program that generates the G-code so I can make changes to some parts of it so my part program will have the changes built into the G-code txt file and I won't need to hand edit each txt G-code fole to get it to run as I want. I just realized the .cnx file I sent was my mistake. I renamed the the Mach3 post to Boss6I hoping it would load into my cad program, but it did not. I meant to attatch this file Boss6I.cnx I will now attatch it to this posting. Sorry for the mixup.
-
OK that one is more like it.
SO what is it that you wanted to change ?
(;-) TP
-
I would like to have the correct startup codes. Mach3 does not want G75 and it does not want the period as the first character in the first line. I would like to add the segment names for the different cycles, and I need to have the correct end commands that retract Z and return to the tool change location. There might be other things I will want to edit in the future. I need to know where to go to edit the post variables to make it happen. I want the post to be compatable with my Mach3 controler.
-
As far as just modifiing things like the startup block that is very easy add or subtract what you want. The canned cycles are already defined. Being that you are dealing with a VERY old CAM program version wise it may NOT support the full aspect of a modern day CNC controller. In that case you will be very limited as to the full support of Mach3.
But it looks to have all the low end features that are required to build parts. It just may be limited to machining features.
Without having full knowledge of the CAM program it will be very hard to prove or disprove that it can handle MAch3 fully. I suggest you email EZCAM and ask them IF your version can handle such things. IF not then time to move on to a modern version of CAM. If it is possible then ask how to go about it. Perhaps they still have documentation of the post system used by that version of Ezcam.
Just a thought, (;-) TP
-
I appreciate your responses. If I wanted to try to edit the post processor, Which file would I need to edit? Is it the .cnc or .cnx file? The .cnx file is easile opened with wordpad, but the .cnc file has a lot of unreadable entrys. When I post a new part program, I load the Boss6I.cnc file into my CAD program to generate the G-code, so I don't know what the purpose of the Boss6I.cnx file is for.
-
You can try editing the readable file. Try just making 1 simple change at first then save and test. If that works then have at it.
Remember to ALWAYS save the original file away safely and only edit a copy. Also do not delete any symbles you see in the file as they may be neccesary for the file to run properly.
(;-) TP
-
I will give it a shot and let you know what happens. I am just wondering how changes to the .cnx file has any affect on the .cnc file. Thanks for your efforts in trying to help me.
-
I did some editing in the .cnx file and had both files in the same directory when I loaded the post to my CAD program, but it had no affect on the G-code produced, so I guess I need to somehow find a program that can display the .cnc file in normal text so I can edit that file to achieve the changes. Any ideas?
-
That won't happen. It is compiled code. I would think somewhere in the Cam program there is a feature to compile the Posts IF that is what it needed.
I have never seen one that ran compiled Post code but it is possible.
(;-) TP
-
I finally found the MBUILD program that I used many years ago. I want to have a Z up movement at the end of the program before any X or Y move. The post shows the program end as: {N<SEQ>}<MOTION>X<X-CHANGE>Y<Y-CHANGE>M2<EOB> Is that what I want, or do I need to add a Z move? If so, what is the correct input?
-
TP,
I figured out that the cnc file is the postprocessor machine file and the cnx file is the text document file that shows the format information contained in the cnc file. I am now able to edit the cnc file with MBUILD. Based on the formats shown in the cnx file, can you give me the correct format for including segment name comments and the correct program end with Z up move? If so, then I can edit the cnc file to include the changes.
-
Just guessing here but the normal Z sequences are Zsurf, Zclear, ZRapid.
I would think that this may work
{N<SEQ>}<MOTION>Z<ZRAPID><EOB>
{N<SEQ>}<MOTION>X<X-CHANGE>Y<Y-CHANGE>M30<EOB>
-
Thanks. I will try that and see what happens. The Boss6I post is about 99% compatable with mach3, so with a few tweeks, I should have a nice post.
-
That program end worked great. Thank you. I will try my hand at doing some editing of my own now that I see some of the logic involved. I guess that is the best way to learn. I thank you for sticking with me through this problem.
-
YOU are welcome you did all the work (;-)
(;-) TP
-
I have a post that has the following program end code. What does the D0 entry do?
PROGRAM END FORMAT:
{N<SEQ>} G0 Z0 D0 M5 M9<EOB>
{N<SEQ>} <MOTION> {X<X-CHANGE>} {Y<Y-CHANGE>}<EOB>
{N<SEQ>} M30<EOB>
N9999 (END,PROG)<EOB>
%<EOB>