[viz]

Attached all my system settings, there will be in "Parameters" directory all parameters list and also you can check Macros. In your video it's so easy to write coordinates for tools. Don't understand why in my machine there is no ATC SET menu.

[mikeDK]

I don't see any difference in your list compare to mine. maybe you need to change the macro or upgrade software on your controller

[viz]

The main problem is that the manufacture who made this CNC machine is not answering any more after they sold it So now i am in trouble with the tools, don't know what to do.

[savarisam]

sir i am using for nc studio 4.5.53 the problem is when nc studio open automatic moving for axis how to solve the problem

[serum]

how did you make a backup of your system? did it involve a keyboard? I just found this PDF online for the Syntec controller;

[serum]

Does anyone know what the macro of an inline ATC for a MA6 looks like? My machine comes with an 8 pcs atc, but it would be handy to add a few more slots. (don't have the machine yet, fist payment has been made though, anxiously waiting for the machine

[Frankmali17]

Hello Serum,
Did you get your SYNTEC Controlled machine?
Did you perform the procedure in the PDF you attached?.. Where did you get the PDF?

As far as I know, when you turn on SYNTEC 6MA or 6MB, if you go to "settings" or "Maintenance" menu.. you will find options about backing up. I backup to a USB drive...
It should copy your macros onto the drive.. I think it makes a "zip" file.

Let me know how it worked out

FrankMali17

[Frankmali17]

Hey Viz,
Did you have any luck solving the problem with your tool change positions?
I Have a 6MB machine, and had to use the G991T(tool number you want) process, and reteach my entire machine when I got it.

I also didn't have an ATC SET menu...

HEY mikeDK.. do you have maybe a 6MD controller? This is the next level of hardware, beyond 6MA or 6MB?

Frankmali17

[Frankmali17]

:cheers:
Hello Everyone, It seems like we can all benefit from sharing information About SYNTEC Controllers.

There is much to be said, So I hope to get your feedback and any comments, So that we may all learn from each other.
It seems very clear to me after using a SYNTEC machine for about 2 years.. the it is a Very capable system, based on my experience and all research, but SUPPORT from SYNTEC is NON-EXISTENT, or very very very poor.

SO after the manufacturer of the machine gets it to you.. (and they are the only ones SYNTEC seems to be interested in talking to), you are often left on your own.
I found the manufacturers, (and many of them now just copy or rip-off what their larger-wiser competitor machine-maker did) don't often have as much knowledge of the system and it's capabilities, and are often just repeating your questions.
They get basic scripts and macros and ladders, and copy hardware setups, and hope it works... after the sale, they don't seem interested in effort to further expand, configure, or develop the product they just sold you.

Am I right so FAR?

FrankMali17
to be continued....

[Frankmali17]

HERE is what I learned and observed and research (in my off-time on available evenings) My machine is a SYNTEC 6MB and I have an 9KW HSD ATC Spindle, and two rows of 8 tools each (linear tool fork setup)

6MA is 3 axis control, 6MB is 4 axis control, 6MD is like 6 or more axis, larger screen, more power. BUT they all run the basic systems.

These controllers, like Mach3, LinuxCNC, etc.. have some basic, or advanced hadware/software that can be configured in many, many different ways by the machine maker.. and therefore all of us have a hard time knowing or helping each other...
There are PLC Ladders, Macros, and other parts of the SYNTEC system, that are customized by each machine maker.

I have studied quite a few examples of all of these.

I should state that While I am not an expert, I have modified and setup my own Post Processors, with my own machine, and run it successfully.

The BiGGEST Problem is Lack of English Documentation (with accurate info) or access to it. and SYNTEC doesn't seem interested in my emails or phone calls. They now have one Representative here in USA.. california, but he doesn't respond after first time I actually got a hold of him... even though I told him I want to buy additional I/O boards to expand my controller.

THE SECOND, is that for PLC LADDERS, etc.. you need software for your PC.. to open and try to modify these... and of course if you can somehow get it.. (i DID) good luck finding manuals in ENGLISH..

Tool changes seem to be run by T0000 macro... which is activated by the PLC when it sees a M06 Command in the code you are running.

I notice that SYTEC manufacturer provided some basic versions of the macro.. and your machine maker then goes and modifies it.

What if find very annoying and challenging, is that the syntax is a bit confusing, and a lot of the variables don't make much sense.. especially when they are called something like " #461" instead of "{desired too}"
So when you see things in your macro as " #50:=#16 " You are like "what the hell is that supposed to be?"

of course there is a format for comments "//comment" but mine are in chinease.. and google translator is a life saver, but often I see the chinease author wasn't interested in you knowing what he wrote.. or intended to do.

Without documentation, proper comments or notes.. I have to reverse engineer just what the hell they did and coded.

I can report that My efforts have led me to study the "G991" macro, and "T0000" macro, and I'm writing in my own english comments and explainations.

MY GOAL is to add to my 16 tool positions, and enable my non-functioning F4 button, work light, coolant, mist, etc...


DO ANY OF YOU HAVE ANY info or manuals, or software to share?
DO ANY HAVE other questions?

MAYBE WE CAN HELP Each other.

[cncjunky2011]

Hi guys,

Did anyone manage to get a copy of the working Post Processor for Vectric Aspire from SyntecLee please? I have contacted him but I don't think he is active on here anymore.
If anyone has the file he was using to share I would be very grateful.

Thank you.

[gfacer2]

Hi guys,

Did anyone manage to get a copy of the working Post Processor for Vectric Aspire from SyntecLee please? I have contacted him but I don't think he is active on here anymore.
If anyone has the file he was using to share I would be very grateful.

Thank you.

Here is my version of a vectric post for a syntec 6md (but Ma/Mb should be same). I also have the application manual (ie installation manual -its useful but its not well done for english at least).

Cut and paste below:

+================================================
+
+ Fanuc 16M Vectric output configuration file modified for Syntec 6m series with ATC
+
+================================================
+
+ History
+
+ Who When What
+ ======== ========== ===========================
+ Mark 22/07/2008 Written
+ Mark 07/09/2010 Added Safe Z definition
+ LRD 01/03/2015 Modified for XYZ Syntec 6MA
+ GFacer 03/14/2016 Changed to Omni Syntec 6m series
+ ===============================================

POST_NAME = "Omni Syntec 6m ATC Arcs V2.5 (mm)(*.nc)"

FILE_EXTENSION = "nc"

UNITS = "MM"

+------------------------------------------------
+ Line terminating characters
+------------------------------------------------

LINE_ENDING = "[13][10]"

+------------------------------------------------
+ Block numbering
+------------------------------------------------

LINE_NUMBER_START = 1
LINE_NUMBER_INCREMENT = 1
LINE_NUMBER_MAXIMUM = 9999999

+================================================
+
+ Formating for variables
+
+================================================

VAR LINE_NUMBER = [N|A|N|1.0]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR FEED_RATE = [F|C|F|1.1]

+-----------------------
+ TOOL MOVES IN X Y Z
+-----------------------
VAR X_POSITION = [X|C|X|1.4]
VAR Y_POSITION = [Y|C|Y|1.4]
VAR Z_POSITION = [Z|C|Z|1.4]

+-----------------------
+ ARC MOVES
+-----------------------
VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.4]
VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.4]

+-----------------------
+ HOME TOOL POSITION
+-----------------------
VAR X_HOME_POSITION = [XH|A|X|1.4]
VAR Y_HOME_POSITION = [YH|A|Y|1.4]
VAR Z_HOME_POSITION = [ZH|A|Z|1.4]

+-----------------------
+ Z SAFE POSITION
+-----------------------
VAR SAFE_Z_HEIGHT = [SAFEZ|A|Z|1.4]

+================================================
+
+ Block definitions for toolpath output
+
+================================================

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER
+---------------------------
+ ORIGINAL
+---------------------------
+"o0001"
+"( [TP_FILENAME] )"
+"[N] G91 G28 [XH] [YH] [ZH]"
+"[N] G00 G21 G17 G90"
+"[N] G00 G40 G49 G80"
+"[N] G71"
+"[N] T[T] M06"
+"[N] G00 G43[ZH]H[T] M8"
+"[N] [S] M03"
+"[N] [XH] [YH] [F]"
+---------------------------

+---------------------------
+ MODIFIED
+---------------------------
"%"
"( [TP_FILENAME] )"
"[N] G54"
+"[N] G00 [XH] [YH]" edited out start at home GF Note added for cnczone - it is apparently good to add some position here even if it is just a small move, so the machine realizes where it is.
+ My brother was using this post and found that for a file that was supposed to start cutting at x:0 y:0 and on the line, it just went down and started the cut even though this post ends the
+ cutting at the back of the table.
"[N] T[T] M06"
"[N] M03 [S]"
"[N] G04 P1000"
"[N] G43 H[T]"
+---------------------------


+---------------------------------------------------
+ Commands output for rapid moves
+---------------------------------------------------

begin RAPID_MOVE

"[N] G00 [X] [Y] [Z]"


+---------------------------------------------------
+ Commands output for the first feed rate move
+---------------------------------------------------

begin FIRST_FEED_MOVE

"[N] G01 [X] [Y] [Z] [F]"


+---------------------------------------------------
+ Commands output for feed rate moves
+---------------------------------------------------

begin FEED_MOVE

"[N] G01 [X] [Y] [Z]"

+---------------------------------------------------
+ Commands output for the first clockwise arc move
+---------------------------------------------------

begin FIRST_CW_ARC_MOVE

"[N] G02 [X] [Y] [I] [J] [F]"

+---------------------------------------------------
+ Commands output for clockwise arc move
+---------------------------------------------------

begin CW_ARC_MOVE

"[N] G02 [X] [Y] [I] [J]"

+---------------------------------------------------
+ Commands output for the first counterclockwise arc move
+---------------------------------------------------

begin FIRST_CCW_ARC_MOVE

"[N] G03 [X] [Y] [I] [J] [F]"

+---------------------------------------------------
+ Commands output for counterclockwise arc move
+---------------------------------------------------

begin CCW_ARC_MOVE

"[N] G03 [X] [Y] [I] [J]"


+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------

begin TOOLCHANGE

"[N] M5"
"[N] G04 P5000"
"[N] T[T] M06"
"[N] G43 H[T]"
"[N] M3 [S]"
"[N] G04 P5000"

+---------------------------------------------------
+ Commands output for a new segment - toolpath
+ with same toolnumber but maybe different feedrates
+---------------------------------------------------

begin NEW_SEGMENT

"[N] G00 [SAFEZ]"
"[N] [S] M03"
+---------------------------------------------------
+ Commands output at the end of the file
+---------------------------------------------------

begin FOOTER

"[N] G00 [SAFEZ]"
"[N] G80"
"[N] M09"
"[N] M5"
"[N] G53 Z0"
"[N] G00 X800.00 Y3125.00"
"[N] M21"
"[N] M23"
"[N] M30"
+ moved finish position at far end of table for loading and unloading - your machine may need different figures or revert to old footer for home position GF
"%"

+----------------------
+ OLD FOOTER
+----------------------
+"[N] G00 [ZH]"
+"[N] M09"
+"[N] G00 [XH] [YH]"
+"[N] M17"
+"[N] M30"
%

[cncjunky2011]

Hi,

Thank you very much for sharing this, it is greatly appreciated.

We have a carousel machine from Philicam but we are having problems getting any support whatsoever from them. I have contacted Vectric who are very helpful and I am hoping we can get the PP to work so we can use their software.

Thank you once again for taking the time to share this, it's much appreciated indeed.

JJ

Here is my version of a vectric post for a syntec 6md (but Ma/Mb should be same). I also have the application manual (ie installation manual -its useful but its not well done for english at least).

Cut and paste below:

+================================================
+
+ Fanuc 16M Vectric output configuration file modified for Syntec 6m series with ATC
+
+================================================
+
+ History
+
+ Who When What
+ ======== ========== ===========================
+ Mark 22/07/2008 Written
+ Mark 07/09/2010 Added Safe Z definition
+ LRD 01/03/2015 Modified for XYZ Syntec 6MA
+ GFacer 03/14/2016 Changed to Omni Syntec 6m series
+ ===============================================

POST_NAME = "Omni Syntec 6m ATC Arcs V2.5 (mm)(*.nc)"

FILE_EXTENSION = "nc"

UNITS = "MM"

+------------------------------------------------
+ Line terminating characters
+------------------------------------------------

LINE_ENDING = "[13][10]"

+------------------------------------------------
+ Block numbering
+------------------------------------------------

LINE_NUMBER_START = 1
LINE_NUMBER_INCREMENT = 1
LINE_NUMBER_MAXIMUM = 9999999

+================================================
+
+ Formating for variables
+
+================================================

VAR LINE_NUMBER = [N|A|N|1.0]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR FEED_RATE = [F|C|F|1.1]

+-----------------------
+ TOOL MOVES IN X Y Z
+-----------------------
VAR X_POSITION = [X|C|X|1.4]
VAR Y_POSITION = [Y|C|Y|1.4]
VAR Z_POSITION = [Z|C|Z|1.4]

+-----------------------
+ ARC MOVES
+-----------------------
VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.4]
VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.4]

+-----------------------
+ HOME TOOL POSITION
+-----------------------
VAR X_HOME_POSITION = [XH|A|X|1.4]
VAR Y_HOME_POSITION = [YH|A|Y|1.4]
VAR Z_HOME_POSITION = [ZH|A|Z|1.4]

+-----------------------
+ Z SAFE POSITION
+-----------------------
VAR SAFE_Z_HEIGHT = [SAFEZ|A|Z|1.4]

+================================================
+
+ Block definitions for toolpath output
+
+================================================

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER
+---------------------------
+ ORIGINAL
+---------------------------
+"o0001"
+"( [TP_FILENAME] )"
+"[N] G91 G28 [XH] [YH] [ZH]"
+"[N] G00 G21 G17 G90"
+"[N] G00 G40 G49 G80"
+"[N] G71"
+"[N] T[T] M06"
+"[N] G00 G43[ZH]H[T] M8"
+"[N] [S] M03"
+"[N] [XH] [YH] [F]"
+---------------------------

+---------------------------
+ MODIFIED
+---------------------------
"%"
"( [TP_FILENAME] )"
"[N] G54"
+"[N] G00 [XH] [YH]" edited out start at home GF Note added for cnczone - it is apparently good to add some position here even if it is just a small move, so the machine realizes where it is.
+ My brother was using this post and found that for a file that was supposed to start cutting at x:0 y:0 and on the line, it just went down and started the cut even though this post ends the
+ cutting at the back of the table.
"[N] T[T] M06"
"[N] M03 [S]"
"[N] G04 P1000"
"[N] G43 H[T]"
+---------------------------


+---------------------------------------------------
+ Commands output for rapid moves
+---------------------------------------------------

begin RAPID_MOVE

"[N] G00 [X] [Y] [Z]"


+---------------------------------------------------
+ Commands output for the first feed rate move
+---------------------------------------------------

begin FIRST_FEED_MOVE

"[N] G01 [X] [Y] [Z] [F]"


+---------------------------------------------------
+ Commands output for feed rate moves
+---------------------------------------------------

begin FEED_MOVE

"[N] G01 [X] [Y] [Z]"

+---------------------------------------------------
+ Commands output for the first clockwise arc move
+---------------------------------------------------

begin FIRST_CW_ARC_MOVE

"[N] G02 [X] [Y] [I] [J] [F]"

+---------------------------------------------------
+ Commands output for clockwise arc move
+---------------------------------------------------

begin CW_ARC_MOVE

"[N] G02 [X] [Y] [I] [J]"

+---------------------------------------------------
+ Commands output for the first counterclockwise arc move
+---------------------------------------------------

begin FIRST_CCW_ARC_MOVE

"[N] G03 [X] [Y] [I] [J] [F]"

+---------------------------------------------------
+ Commands output for counterclockwise arc move
+---------------------------------------------------

begin CCW_ARC_MOVE

"[N] G03 [X] [Y] [I] [J]"


+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------

begin TOOLCHANGE

"[N] M5"
"[N] G04 P5000"
"[N] T[T] M06"
"[N] G43 H[T]"
"[N] M3 [S]"
"[N] G04 P5000"

+---------------------------------------------------
+ Commands output for a new segment - toolpath
+ with same toolnumber but maybe different feedrates
+---------------------------------------------------

begin NEW_SEGMENT

"[N] G00 [SAFEZ]"
"[N] [S] M03"
+---------------------------------------------------
+ Commands output at the end of the file
+---------------------------------------------------

begin FOOTER

"[N] G00 [SAFEZ]"
"[N] G80"
"[N] M09"
"[N] M5"
"[N] G53 Z0"
"[N] G00 X800.00 Y3125.00"
"[N] M21"
"[N] M23"
"[N] M30"
+ moved finish position at far end of table for loading and unloading - your machine may need different figures or revert to old footer for home position GF
"%"

+----------------------
+ OLD FOOTER
+----------------------
+"[N] G00 [ZH]"
+"[N] M09"
+"[N] G00 [XH] [YH]"
+"[N] M17"
+"[N] M30"
%

[gfacer2]

Here is some more information if you want to get your hands dirty in the Syntec controller. I know one person that did get the ladder modified (name escapes me now) but he has not posted a detailed write up on how or what he did.

Anyhow, if I can get these to attach it is a few power point decks for training on the PLC and the application manual (ie programming manual). Looks like I will need to save the PPT files into PDF's

[gfacer2]

OK - Hopefully basic PLC powerpoint (now PDF):

[gfacer2]

And Advanced:

[cncjunky2011]

Excellent, extremely helpful.

Thank you very much.

[mikeDK]

I got an email from Graham who ask me to write a little about how I change the ladder file on Syntec controller.

for starters, you need to install MLCEdit to change the ladder, once installed you simply make a complete backup of your controller or for the trained ones just get the ladder backup. then open the ladder file with MLCEdit, name of file is "cnc.lad"
now you can edit the ladder file.

I have on my own controller change the Air Blow button to work with M8/9
and found out that M175/176 is the dust cover up and down.

I used this manual form a Chinese site, it is in english and it shows an old software, but the methode is the same.


LINKS:
https://wenku.baidu.com/view/fa5ea30...102d220e5.html (manual)

https://www.dropbox.com/sh/ryh66kuv5...t1F_Klaua?dl=0 (MLCEdit software)

[gfacer2]

I did try again, and it looks like I can open the editor. It seems fairly straightforward to take a button on your keypad that is hooked up to a relay and make a m code for it. I can post a before and after on the ones my vendor edited maybe tomorrow.

Maybe I'll try those extra options I've been thinking of (reducing air consumption of the spindle when resting and coolant).

Sent from my LG-D852 using Tapatalk

[Frankmali17]

I'm attaching my "cleaned up" post Processor for VCARVE PRO

I had to Change the file Extension from ".pp" to ".txt" so that the CNCZONE would allow it to upload.
You need to change it back to use it.

I have a linear tool holder.. for my HSD ATC Spindle...
But quite honestly, that may not matter.. as the tool change procedure is managed by the controller once it sees the "M06 T#" request.

NOTE: I decided to use G53 coordinates.. as my "home" referance..

So if Vectric when I design, the home parameters, and I enter X24 and Y96... it will start or Park there.. regardless if I use a works offset...
You will know what I mean if you look at the PP and are familiar with using the G53 command.

GOOD LUCK .. let me know if any of this helped someone.