Hey Mike and Serum...
This is quite hard to explain in a few words but I will try.
Please test this carefully!...
Please understand that there is a LOT of things happening in the MACRO... while the PLC is doing a lot of other things. AND your machine maker can configure syntec in their own way.. .and can create their own variables.
The Better you can understand it all.. the more this will make sence. Always Test carefully, As I cannot take responsibility for unforseen errors.
I'm attaching a picture to help.
In the beginning of your macro You need to add some lines that will store your mm/inch mode...
and toward the end, before exiting the macro, you will then "recall" that info.. and put the machine into proper mm/inch mode... to continue running your program correctly.
Also..
look for @460:=1
This is actually putting a value of "1" into Registry bit #60 ... yes #60.. not #460 like it would make sence.
this makes Rapids.. or G00 moves at 50%...
So if you would add "//" in front of it... that would make it just a comment...and Syntec will ingnore it... That's the way I recommend it...
Notice at some point.. there is a command "@460:=0" That's when it makes G00 go back to 100%.
I would try it only on lets say Tool #1... and see if you still think it's a good idea.. after you test it out.
Then you could proceed to modify it for all 8 tools.
Guys,
Thank you for sharing your macro...
I hope to give back to the community.
What has been challenging.. is while I am humble... I feel I have quite a bit of experience... and yet I have spent hundreds of hours studying this SYNTEC system.. to be able to get more knowledgeble of it.
NO Formal training or support is available...
Now I understand why some of this stuff costs like $1000 a day for them to come and help you...
and quite honestly... it takes about a day.. to study a larger macro thoroughly to do more significant changes.
ALWAYS DO A BACKUP of your CURRENT AND EXISTING data.. before loading any modified versions. !
Good Luck.
Mike let me know if my info is making sence to you. I spent about 75minutes on it this evening...
This is the great syntec thread, so don't expect any reply too soon
The card you are looking for is listed on Taobao, i noticed in a movie on youtube that there is a 6.1 revision, but the board is named TB16OUT. if you do a search for that on taobao, there are several offers available.
I would just like to mention that Syntec's USA branch has just recently launched operation. I see communicating overseas has not been ideal, and so if you have any future orders you are trying to place, or any minor support issues, feel free to contact me directly milan.ardeshna@syntecclub.com.tw
I would also like to mention that any complex problems may still have to be sent to Taiwan as we are training new engineers and have many large scale customers, but feel free to ask anyway and I will do the best I can and respond in a timely manner.
It seems there are already many skilled professionals taking initiative on here already so it seems like we are all in good hands.
Yeh, i bought through an agent. Language barrier and alipay. It's something like the Asian ebay, only much, much largers in number of users. I would recommend using an agent, since taobao is depending on alipay. Yoybuy seems to be the biggest.
Thanks Frankmali17,
I did as you suggested and inserted // in front of the "@460:=0". That works great. You sir, are AWESOME.
I am not yet comfortable with your suggestion to do your quote- "In the beginning of your macro You need to add some lines that will store your mm/inch mode...
and toward the end, before exiting the macro, you will then "recall" that info.. and put the machine into proper mm/inch mode... to continue running your program correctly."
I don't quite understand your thumbnail.
Also, I would like to add that I created a program like this:
O0001
G71
M6T1
G70
M30
I created this just to change tools, rather than having to type this into MDI every time I wanted to change tools manually, as I could not just MDI T1M6.
I noticed there is a few seconds of lag in the program, so that I have to wait about 3 seconds after the tool change is done before I switch to jog mode.
What was happening is that I would change tools and switch to jog mode before letting the program complete. Then the machine was in metric mode and I had to go back into settings and change it again to inch mode.
Hopefully your suggestion of inserting the mode change in the macro will take care of this issue.
Here is my current macro. Could you highlight where you are referring to?
% @MACRO
WAIT();
//ZÖᰲȫ¸ß¶È²ÎÊýΪ2823
//YÖá»»µ¶Ç°ÖõãλÖòÎÊýΪ2822
//»»µ¶×Ô¶¯¶Ôµ¶XYλÖÃΪ²ÎÊý2841 Óë²ÎÊý2842
//******************************************
//ÅжÏÄ¿±êµ¶ºÅ²»ÔÚ·¶Î§ÄÚ¾ÍÌ ø³ö»»µ¶macro
IF (0 = #1036 OR #1036>8 OR #1036<0 ) THEN
M99;
END_IF;
WAIT();
I believe he means something as followed. The mm/inch is stored by the controller automatically along with a few other things you may want backed up and then recall after a tool change.
start your macro by taking whatever your controller is using.
The macro will likely have to change these things in the process of the tool change. you want to reapply what was there before the tool change after the tool change is done by doing the following at the end of the macro.
G#31; // Reply to interpolation mode
G#32; // Reply G91 or G90 state
G#34; // Reply machining feed mode 94/95
F#33; // Reply feed
Ill try to answer simple questions and feel free to pm if you need further assistance that cant be discussed on a forum.
Thanks Syntecengineer. I am going to have to take some time and try to understand this. I realize the necessity of recording the data and the reinstating the data, but not sure how to go about it.
On a different question, I have not been able to figure out how to start a program from a tool change. I have been having to start each program from the beginning. It seems like it would be simple, but I can;t seem to figure it out.
Say I run tool 1 and 2 completely through a program, and just want to re-run tool 2 with an offset, how can I toggle down in the program to start at tool 2?
I have a Syntec 6MA.
Thanks again. These forums are a big help.
Welcome to cnczone SyntecEngineer! Are you a Syntec employee or an enthusiast? Can anyone point out what needs to be changed to hook up a pneumatic valve to one of the output relays and to control it through an M code?
Hi serum,
I have the same type of output relays as you. I don't know if this helps or not, but I have a couple empty relays and one of them is controlled from the front panel air blow switch. I believe there should be an M code to control the air blow. Would that be any help?
Mike
Hello there Mike...
Where are you from? What are your machine details?.. Size, Spindle, Controller type, Axis Motors, Linear or Rotary?...
About starting your program NOT from beginning.
I believe you have to be in "Monitor" Screen....
(I actually run all my programs in this screen and also open the toolpath preview)
When you are ready to run the program.. (Auto Run has to be turned on) and you see the Gcode on the bottom from the beginning...
Use your keypad on the right.... to type in for example: "20" and hit enter...
It should jump down to line 20.. and you should be able to pick up from there when you hit Cycle START...
Remember though.. line 20.. isn't necessarily N20.. or N020.. It will be actually line number 20.
I believe if you press T2.. for example.. instead of a line number... it will search for where T2 shows up...
If you want to just to a line in your code with a prefix of N1120.... you would type N1120
Serum , Mike...
Are you able to read/modify your Ladder?... And understand it?...
That is a touchy, touchy, thing.... but that is where you would have to map out the correct inputs, etc.. and assign to an output..(relay) and also create a few conditions/variables.
Remember, the Ladder is how we program the PLC inside Syntec, to configure how inputs/outputs are configured.. but also create logic, for how/when/if what should or shouldn't happen SAFELY...
Mike, about your macro...
That is a long attachment :-)
It would take a long long time for me to filter through it.. but here is something I noticed.. and was trying to say before...
Look at your file... the 3rd line from the bottom says "G@105"
What its trying to do is say.. G"Variable105"... so if you want go to inch mode.. it would need to plug in the variable the represents the 70... for G70
Remember... this macro should work weather you started in Inch or mm machining mode...
at the top of your macro, find these lines:
@104:=#1036; //´¢´æ¼Ó¹¤³ÌʽT_codeÏ´ïµÄÄ¿±ê µ¶ºÅ
@103:=#1004; //´¢´æ½øÈë»»µ¶MACROÇ°µÄG91/G90״̬
You need to add this line, right bellow the two:
@105:=#1010;
This is going to look at your machine's current mm/inch mode.... record it to that @105 variable... and then recall it at the bottom before you exit out the macro...
"#1010" is a modal variable for mm/inch machine status...
Of course you could have just changed that "3rd from the bottom line" to G70... but if you ever ran in mm mode.. you would always end up in inch mode after the tool change.. and OOPS!
So,that would be the first thing I would try in your T0000 macro..
Like I said.. it will take really long to look for any other errors...
It has taken me a long time.. lots of Research.. and countless hours at machine and computer, reverse engineering what is happening.. to be able to start getting more comfortable with all this.
Yes I am both the engineer and rep for the U.S. branch of Syntec. Sorry for the difficulty on ordering your extension parts, next time you can just pm me for my contact.
Also the local variables are ideal since you only need to use an Rbit when you want to map it to the ladder. If its never an issue outside of the macro local is fine.
Serum as Frank said, to produce M codes to control relays you will have to use a ladder to map any unused M number to the specific O bit that controls that relay. that was likely wired by your machine maker.
Quick question. Are you guys machine makers or the end users of these machines? Direct customers of Syntec for controllers or has it just came on the machine? Im just curious since you guys seem to be developing your own programs.
Great! Nice to see some support from Syntec on this forum! I know it's greatly appreciated by the users here (me included). I'm an end-user, and I think all the Syntec users here are happy with your support and help.
Well, I spent most of the day playing with the tool change macro and I think I finally have it all working properly. I have to give you guys credit and kudos. I don't know how you guys can look at the macros and ladders without getting totally confused. I was for most of the day and actually still am. I translated the comments from Chinese to English and that helped somewhat. I ended up putting a G71 at a few places in the macro rather than have the machine refer back to a register. I was getting too confused trying that. I first did as Frank suggested and it seemed to work and return back to inch mode only if I did the tool touch probe routine. I tried modifying that somewhat, but no luck. Anyway, if we ever switch to start running metric programs, I will just load the original tool change macro. I also was able to start a program after a tool change as Frank suggested. Thanks so much to everyone on this forum.
I took the original machine table off and replaced it with an 1-1/4" thick mic6 aluminum tooling plate. Machined hole patterns and slots to mount different attachments and Kurt vises. Made a horizontal head to mount the spindle on. That worked well. We had to thread some 3" cpvc pipe that was too long for the lathe, so we made the horizontal head and thread milled the pipe on the router.
I like the syntec control because it is very similar to fanuc. Very robust along with the yaskawa servos.
There were several issues with the mechanical aspects of the machine, but those have been worked out.
I think I will use the machine a ton more now that it has the tooling plate top. It was a real hassle to mount anything to the vacuum table.
If I get a chance , I will try to post some pics next week.
Mike
Hey Mike...
Pictures would be great.. and would help to understand better what you are describing.
I'm glad that the info on the Macro helped...
I would have to look closer.. but Between the variable in the begining, and recalling it at the end... there is some more that may be needed...
You machines tool macro probably looks to confirm, that you pressed the button to request tool measuring.
Otherwise, it probably exits the program..
It would need to recall the mm/inch mode right before it exits the tool change.. and skips tool measuring.
I looked at it again...
I'm sure you used a translation for the Chinese comments.. and some of it doesn't make sense... :-)
I That is why it is a real project, isn't it.. When google says "knife" it's actually more accurate to say "cutter" he,he,he...
Anyway... More on what I was saying before...
Notice that at some points in your macro.. you will see an m-code... M176.
That indicates that you are completing/exiting the tool macro.. and lowering the dust hood...
You also see: G@103;
This is where you are recalling if your were in G91 mode.. or G90 mode...
right bellow that.. is where you would want to insert the line:
G@105;
and then it tells it to change Rapids back to 100% by saying: @460:= 0;
Let me know if that works...
Hopefully this info.. lets you find the few spots the macro may exit.. and you can recall your mm/inch mode right before that.
- - - Updated - - -
Good luck,
and I hope to see what you have done with you machine...
Take plenty of pictures with your even with your phone.. if that is easier to share.