Post Processor for Intelitek proLIGHT 1000 CNC Milling Center - Fanuc?

[Anonymous]

I'm a highschool student trying to get my school's Intelitek proLIGHT 1000 CNC Milling Centers up and running. They work with the old software that came with them, but they're really out dated and unintuitive, so I'm trying to use HSMXpress to create the tool paths to then send to the machine.

The problem I'm having is with the post processor. None of the post processors that I have tried are compatible with the software that runs the .NC programs for mill. The .NC files are either completely unable to be used in the software, or they try to move the machine into a position it cant go to (one tried to move the X-axis to -37 or something, which is alot futher than the X-axis can travel).

This website has some info on the machine I'm trying to use. http://www.great-lakes-training.com/CNC_Mill_PLM1000.html

The site says "It features an intuitive Windows 95 software interface and conform to industrial EIA, ISO, Fanuc, G and M code standards." but I've tried all the Fanuc post processors that come with HSMXpress with no success.

Any suggestions of what I should do? Your help would be greatly appreciated.


Thanks

[fonsecr]

I made a preliminary post now. It needs some testing before I'll make it public. Just ask if you want to test it.

You can turn on/off tool changer using the "useToolChanger" setting in the post dialog. Default is enabled.

The CNC control is a using a mixture of the Fanuc and RS-274 styles.

[XanderLuciano]

Martin Krogulec wrote:
You should have "Post processor manual" in Menu Start > Programs > HSMXpress. There is a lot of stuff You need:)

I looked through the folder(manually and using the built in search function) and did not find a file. I am using HSMworks not xpress, would this make a difference? Either way would u mind posting the file for me to go through? Thank you.

And Rene, Thanks for the post, I will be sure to check with all types of toolpathing in the upcoming days(Busy with the CSWP currently) and will let you know if I run into any errors. Also seeing as you are more of the expert here, for what I did with the post(crude as it was) was that a "good" solution to the error? Obviously its been working for our machines for the longest times without errors, but wanted your opinion on it.

[fonsecr]

You should see the "Post Processor Manual" option under "HSMWorks" in the Windows start menu.

PS. Your post changes were ok but they were based on the generic Fanuc post which does have some differences to the Intelitek control. My preliminary post is made specifically for the Intelitek control - so once the post has been verified that should be used.

[XanderLuciano]

René Fonseca wrote:
You should see the "Post Processor Manual" option under "HSMWorks" in the Windows start menu. PS. Your post changes were ok but they were based on the generic Fanuc post which does have some differences to the Intelitek control. My preliminary post is made specifically for the Intelitek control - so once the post has been verified that should be used.

Well I found it haha, just wasn't looking good I suppose. And good to hear about my solution. At least I know I'll be able to edit things when I need a quick fix haha. Time to start reading up I suppose!

[Anonymous]

@ René Fonseca

The preliminary post you sent to me didnt work. When I tried to run a program the machine would move the Z-axis all the way up, and then start to move the X-Axis all the way to the right (In which I would then hit the e-stop since if I let it do that it would knock the PC over haha, gotta move that) So basically it is doing the same thing as when I tried using just a generic Fanuc post.

on the other hand,

@ Xander Luciano

Your updated post works like a charm. Spindle works and I able to start running programs and cutting up some machining wax  ;D. Can't wait to start making more complex things. And like you said, I'll try and start learning G and M codes so I'll actually understand what I'm doing.

[XanderLuciano]

Max Meaker wrote:

@ René Fonseca The preliminary post you sent to me didnt work. When I tried to run a program the machine would move the Z-axis all the way up, and then start to move the X-Axis all the way to the right (In which I would then hit the e-stop since if I let it do that it would knock the PC over haha, gotta move that) So basically it is doing the same thing as when I tried using just a generic Fanuc post. on the other hand, @ Xander Luciano Your updated post works like a charm. Spindle works and I able to start running programs and cutting up some machining wax  ;D. Can't wait to start making more complex things. And like you said, I'll try and start learning G and M codes so I'll actually understand what I'm doing.

Sweet to hear dude! So glad I could get it to work properly for you. 😄 (Also makes me feel skilled that my post worked so well haha)

And the G and M codes are too hard, you really just need to learn the common ones so when you look through a post you know what its doing and why it is/isn't doing something(like in your case it wasn't spinning so I added an M03 to start spindle and the beginning of the post.) Also out of question, does the spindle stop? I don't think I put a spindle stop int the code but it should stop when it reaches the end of the program. Let me know if you have issues with that.

[fonsecr]

Ok.

I would appreciate some more information on the post, though. So if you happen to find some free time you can try to post a simple NC program and add comments in the program which tell what is wrong or where the program fails. Then I can check if it is because something needs to be changed in the post or because something is unsupported on the control for which we should add a setting in the post.

Thanks.

[Anonymous]

@Xander Luciano

Yes the spindle does stop at the end of the program.

@René Fonseca

It's hard for me to find time on the machine right now since I have AP testing. But when I get a chance I'll try your post again and let you know more specifically what doesnt work.

[XanderLuciano]

@Max Perfect! Great to hear.

@René Like I said before the machine doesn't like the G28 reference code. The most optimal way to return home would be to retract the Z then move X and Y by a G00. As for the part of the post that screws it up here is the code:

%
; 1
; T2  D=0.125 CR=0 - ZMIN=-0.155 - flat end mill
N0 G90
N1 G17
N2 G70
N3 G28
N4 G53 G0 Z0
; 2D Adaptive1
N5 T2 M6
; 2 Flute Flat Endmill
N6 S5000 M3
N7 G54

N3 G28 would be the line to mess it up. Ill do further testing on my machine tomorrow and see if I can give you a more detailed result and if any other codes work better. Is the G28 even needed? In the post I edited without the G28 it works just fine. I believe this is also caused by the way in which the machine handles the home position.

[fonsecr]

The manual states that G28 goes to home position and also calibrates the axes. But apparently it is not always supported.

I added a post property called "useG28" which is disabled by default. See attached post.

[Anonymous]

 Hi,

I am trying to generate g code with Fusion 360 for an old proLIGHT 1000 CNC mill. The machine is controlled by an (outdated) DOS software running on a Win 95 PC. I tried the generic and customized Intelitek post processors that i found on this thread, but the nc program generated failed to run ( i got error for unsupported codes such as G53/G54). I think the reason is the DOS control software, which doesn't support as many g-codes as the "newer" Windows one provided by Intelitek (attached is the list of G & M codes supported according to the user's manual).

Does anyone have a compatible post processor that may work for my setup? 

Thank you in advance,

Stavros 

[jusalgado36]

Hello everyone, not sure if this thread has some active users but would this post processor work with a super prolight. it is the newer version of the original prolight 1000. I do not have any documentation of file example. Thanks in advance for any help. @fonsecr 

[fonsecr]

The posts attached here are quite old. Have a look at https://cam.autodesk.com/hsmposts?p=intelitek and see if that can be used. Changes might be required though.

There is a manual here which might help https://downloads.intelitek.com/Manuals/CNC/Discontinued%20Machines/proLIGHT_1000_WIN_Manual.pdf