SYNTEC post processor

[info]

Hello,

I have a question regarding post processors. I am planning to buy profesional cnc machine which is controled via taiwanees SYNTEC control system. I am using Fusion 360 as a main CAD software and I really dont want to switch to other softwares. My question is, do any one have experience with SYNTEC controll system and neccesary post processor for this system? Does the fusion contains any usable post processor which is compatible with SYNTEC control system? Also does it support tool changing functions?

Thank you very much for any suggestions I dont have any experience with this so far I was only using MACH 3 with fusion and I would really like to maintain Fusion 360 as a CAM software.

Ondrej CZ

[LibertyMachine]

If you can get a sample program that would have run on that machine or control, we should be able to match it up to something similar in Fusion. Once we find a similar post, we can do some small tweaks to get it into a functioning post for your machine

[damincin]

If this is your manual: http://servocontrolsystem.com/main/wp-content/uploads/2015/05/Mill-Programming-Manual-EN.pdf, looks like the only change might be this:

"SYNTEC 900M G code uses RS274D standards, and the only differences with FANUC 0M are G70, G71 respective to G20, G21."

That's a pretty trivial modification.

Dave

[jasonharrelson]

Seriously? I have a Syntec 900T control and have not had an easy time with posting code to my machine. I know someone has a solution, but I'm not sure where to find the resources. I don't see Syntec listed and the Fanuc post is nowhere near what I need. Any advice? 

---

@damincin wrote:

If this is your manual: http://servocontrolsystem.com/main/wp-content/uploads/2015/05/Mill-Programming-Manual-EN.pdf, looks like the only change might be this:

"SYNTEC 900M G code uses RS274D standards, and the only differences with FANUC 0M are G70, G71 respective to G20, G21."

That's a pretty trivial modification.

Dave

---

[jasonharrelson]

From what I have read in the post processor database, it is expected that I select a property type. I have no idea how to do this and there are no instructions? 

This is what is posted on the page...

"Generic turning post for FANUC. Use the property 'type' to switch the FANUC mode A, B, and C. The default mode is A."

I've read everything I can find on posts yet I don't see instructions. 

[LibertyMachine]

[jasonharrelson]

Wow! Thank you! 

I've literally been trying to find that for 1.5 years!!!

[jasonharrelson]

It seems type "C" does not post anything? I cannot get any code using "C" for some reason. 

Is every single step going to be a bug this year? 😉

[LibertyMachine]

There are true bugs and there is operator induced slash incomplete understanding of what is needed. My best advice is this:

You have absolute proven code from your machine, right? You are making parts and all is good, just with another software?

Take that code. Replicate all your models and tool paths in Fusion. Contact your local reseller. Give them your Fusion file and code that you know will be perfect. Ask them for a price on bringing an HSM post up to speed for your needs. I promise you it will be cheaper and easier than pulling your hair out.

Get prices from multiple vendors and go from there.

[jasonharrelson]

Thanks Seth, 

I would have done this 1.5 years ago had it been an option. I don't know who to contact to get a post, but that would definitely be easier than getting stuck every 15 minutes. I could have built 5 trumpets in the time I've tried get through roadblocks just in the past month. I'll look for a reseller and see if this is an option. This is the first I have ever heard that I could get a custom post for my machine outside of Featurecam/Partmaker. 

Btw, I don't use any software to program my machine. It's all done manually, which is ironically very fast. But I need to move everything to CAD/CAM so my team can make edits without crashing the machine. 

I appreciate your guidance!

Jason 

---

@LibertyMachine wrote:

There are true bugs and there is operator induced slash incomplete understanding of what is needed. My best advice is this:

You have absolute proven code from your machine, right? You are making parts and all is good, just with another software?

Take that code. Replicate all your models and tool paths in Fusion. Contact your local reseller. Give them your Fusion file and code that you know will be perfect. Ask them for a price on bringing an HSM post up to speed for your needs. I promise you it will be cheaper and easier than pulling your hair out.

Get prices from multiple vendors and go from there.

---

[LibertyMachine]

@jasonharrelson

Here is a LIST OF RESELLERS

I suspect they have some sort of "territory agreement" going on, but I say to heck with that. Let the best price and service win. You might want to play it quiet where you are from, although I'm sure that will come through eventually. FWIW, I had great post-edit service and pricing through SilverHawk in Florida. I had some rather advanced 4th axis edits to do that were simply over my head.

In the end, you need to make parts, not screw around with a post. Spend the short money and get it done. And if it's not exactly what you are needing, let them know and they will tweak as needed. But, be realistic, in the end; If it doesn't match exactly, but produces a safe and accurate cut each time, it might just be good enough

[jasonharrelson]

Okay, apparently the "C" must be capitalized! Got it Fusion.

[apparatusinfo]

I might just have what you are looking for.  In my case, working on unabling a certain SYNTAC 900t machine with fanuc 31i control.  And after changing  couple of things (see screen shoots) , I came to this( and it seems to be pretty close if not there yet 😞

%
O0099 (FANUC 31I DOSAN)
G21
M110
M24

N1(PROFILE1)
G0 G28 G53 B0. (SUB SPINDLE RETURN)
G28 U0. V0.
G28 W0.
M190
G54
G99 G18 M134
G50 S5000
T0100
(INSIDE CUTTER)
M8
G97 S3130 M3 P13
M110
G0 Z-1.8
X9.3 Y0.
G96 S91 M3 P13
X9.322
G1 X10.576 F0.13
X14.1
G2 X15.9 Z-0.9 R0.9
X14.1 Z0. R0.9
G1 X12.34
X12.295 Z0.007
X12.265 Z0.026
X12.038 Z0.322
G3 X11.9 Z0.694 R1.04
G1 Z9.386
G3 X12.038 Z9.758 R1.04
G1 X12.254 Z10.04
X10.117
G0 X9.3
Z-1.8
G97 S3130 M3 P13
M5 P13
M9

M25
G28 U0. V0.
G28 W0.
G0 G28 G53 B0. (SUB SPINDLE RETURN)
M134
G54 M80

M111
M30
%

[KrupalVala]

Hi Everyone,

We have a SYNTEC control Post Processor. This post has not been released yet but it is available in the beta version. You can download it from here.

Before the machining trial, please test the codes carefully. 

Thanks,

[hansUV3SU]

Hello @KrupalVala many thanks for the advice

I've tried the post processor and it works fine

only one issue: pickup of the tools is not according to the program of my model in Fusion360

as you see in the processed file under here 

the commando for the tools is misleading

%
O1001
(T1 D=12. CR=0. - ZMIN=-20. - FLAT END MILL)
(T3 D=6. CR=0. - ZMIN=-20.5 - FLAT END MILL)
N10 G90 G94 G17 G49 G40 G80
N15 G71
N20 G28 G91 Z0.
N25 G90

(2D POCKET1)
N30 T1 M06
N35 T3
N40 S8000 M03
N45 G54
N50 M08
N55 G00 X39.3 Y210.263
N60 G43 Z15. H01
N65 G00 Z6.
N70 G01 Z-3.8 F333.
N75 G19 G02 Y209.063 Z-5. J-1.2
N80 G17 G03 X42.1 I1.4 F1000.

@KrupalVala do you have any advice what to do to get it right directly from the post processor?

[KrupalVala]

HI @hansUV3SU ,

T1 is first & T3 Is the NeXT tool number.

T3 is preload tool. If we are not calling "T" (ToolNumber) with "M6" (ToolChange) code then the controller gives a command to the machine to Preloads the next tool in ATC not to the spindle.