Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Need a post processor for Syntec EZ3M

k.petersenRJ3MZ
Contributor

Need a post processor for Syntec EZ3M

k.petersenRJ3MZ
Contributor
Contributor

Hello guys,
i need a post prozessor for Syntec EZ3M.
Can anyone help me?

0 Likes
Reply
730 Views
10 Replies
Replies (10)

engineguy
Mentor
Mentor

@k.petersenRJ3MZ 

 

Do you have any sample G Code from your Machine Operators Manual ??

 

I think that it may be ISO Code based so I suggest that you start with a Basic Fanuc Post Processor and see if the control will accept and run a small test program first.

 

1 Like

k.petersenRJ3MZ
Contributor
Contributor

I have a manuel with G Code include. I hope that can help you

0 Likes

k.petersenRJ3MZ
Contributor
Contributor

We have a post processor from our machine.  It works with the program “aspire” from vectric. See the link

0 Likes

seth.madore
Community Manager
Community Manager

The Vectric post processor will not be at all compatible with Fusion, totally different language.

However, what @engineguy says is correct, I'd start with either the Fanuc or Mach3 post. To get to the bare minimum ISO style post, use the RS-274 post


Seth Madore
Customer Advocacy Manager - Manufacturing
1 Like

engineguy
Mentor
Mentor

@k.petersenRJ3MZ 

 

Well, there you have it, choice is yours, either go and get the Vectric software or stay with Fusion and start as Seth @seth.madore  rightly says either the Fanuc or Mach3 Post Processors.

 

I had a look through your Manual and the G codes, look fine (ISO) and as already mentioned earlier you should do a small, simple program and generate some G Code and try loading it into your CNC Machine Control and see if it will work.

You have the full Manual so go through the setting up of your machine carefully and I think either of the already mentioned options will work for you :slightly_smiling_face:

1 Like

k.petersenRJ3MZ
Contributor
Contributor

So, it works ! Thank you yo much for the help :face_blowing_a_kiss: (fanuc.cps)

but i have now two other  (small) problems.


First problem is, i have it all in mm not in inch and my machine broke it up at the simulation.
"N15 G21" is the problem. When I delete it, than it works. Anyone an Idea how i can change it or how i delete it?

 

The other problem is (see the attachment), how can i say, that my wokpiece zero point is by X0 Y0 ?

In the one pic with X=(-2.936,1603.702) Y=(0.000,2933.690) Z=(0.000,39.000) is that what i want, but where can i change it? I cant find it 

 

0 Likes

engineguy
Mentor
Mentor

@k.petersenRJ3MZ 

 

OK, first part, Inch or MM, in your "Manufacture" area go to the top left of your screen and look for the  Units as in the image below, whatever you set there MM or Inch will be output in the code, set to Inch and you will have a G20, set to MM and you will have G21. The Post Processor will output whatever is set here automatically :slightly_smiling_face:

If you are always going to be working in Inches then you cn make Inches the "Default" so you will not have to make any changes again.

 

Change MM to Inch.jpg

 

For seting the WCS point (Corner or Middle) that is done in the Setup, see image below, with the "Box Point" selected as in the image you can click on any of the points shown and that will move the WCS to that location. Then use the same loocation on the Stock on your CNC Machine, they have to be the same for it to work correctly :slightly_smiling_face:

Stock Box Point.jpg

 

 Hope that helps :slightly_smiling_face:

1 Like

k.petersenRJ3MZ
Contributor
Contributor

Thank you the second part works too.

The first part (G21 or G20) dosn´t working.
In the manuel (G Code List) isn´t  G20 or G21. I think i have to delete that every time. My machine has a problem with this G Code. He dosn´t know it :neutral_face:


But, I am so happy, my first test runs good.  :grinning_face_with_big_eyes:

I have now an other question :see_no_evil_monkey:
By the Tool change is in the program "N30 T5 M06, N35 T4"
He change than from T6 to T5 and than immediatly to T4.  Now idea why? I want to change from T6 to T4

What i made wrong ?

 

0 Likes

engineguy
Mentor
Mentor

@k.petersenRJ3MZ 

 

Apologies for the delay, had to go out for a while.

 

First thing, the G20 and G21 are as you rightly say not in the list of G Codes, (I missed that :disappointed_face: ) I have modified a Fanuc Post Processor so that it does not output any G20 or G21 so try the attached .cps file, just save it to your computer and copy it to your Clipboard,  then open your Posting Dialog, select Setup and from the list that wil appear select "Open Folder" and then just "Paste" the new .cps file into that folder, then you need to close the Dialog by clicking "Cancel", now when you re-open the Posting Dialog you will be able to select the new modified Fanuc Post Processor.

which I named Fanuc(3)-SYNTEC so it might be easier for you to find :slightly_smiling_face: :slightly_smiling_face:

 

Second one is that you probably have the "Preload Tool" set to "Yes" (This is the default) so change it to "No" as in the image below and the preload tool will not be output.

Preload tool.jpg

 

1 Like

k.petersenRJ3MZ
Contributor
Contributor

Hey engineguy,
thank you so much for the .cps file and your help. :grinning_face:
I have changed the pre load tool to no.
Now i have to try my first practice test.  I am curious if everyting is works 

0 Likes