Post for Prototrak 1630SX lathe SLX control

Anyone know of a post for the Prototrak 1630SX lathe? It has the prototrak SLX control. Curious if its even possible since the control uses event pages when programming.

Thanks

Ever get this resolved? I recently purchased a TRL 1630SX and have been having a lot of problems getting a proper post processor for using mastercam to program it.

Since you guys are in the Mastercam directory I assume you want one for a version of Mastercam.

I just got one sent to me and I worked all day on Monday with it. Honestly I don't think it is for this Lathe at all. Unless I just don't understand what tool group upper left or tool group lower right is, this post is not for my machine. ProtoTrak is supposed to be able to run G code but I do not get much support from the dealer on this area. He seems to think I can do everything I would ever want to do from the controller.

I am running mastercam-6. If you want it I will send it to you, no promises though.

Lee

This may or may not help.....but on our 1840 VL lathe, I tried for a long time to get a working post for FeatureCam Turn. I followed the instructions in the Prototrak manual which said to use the .GCD file extension if trying to import G code. I got nothing but garbage.

I tried it out with the .CAM extension and everything worked fine.

The control converts the G code to its own event system which can then be edited at the control if need be.

Hope this helps......I had pretty much no luck getting the tech at Southwest to call me back on any of my half dozen attempts for help.

I have been working on this with a guy from MasterCam's education division. It has been a slow painful process but I think we are pretty near to having a post that works reasonably well for standard turning operations. It still throws some odd error messages but runs correctly if you ignore them. It will output a .CAM file which is then converted to SWI's Events system of programming. There are still a couple of quirks however that I have been working around. First if you want to run the spindle speed in constant surface feet mode the post outputs a G50 for max spindle that makes the g code converter choke, so you have to manually delete G50's from you editor. Also, you have to select a home tool change location when you start up the machine, and mastercam also makes you define a home position for each operation. Therefore, you must remember to set them identically in both mastercam and the machine because it will use both which results in some funky maneuvers between operations. Straight threads works O.K. but it totally screws up tapered threading. I intend to make one more attempt with my contact a mastercam to clean up these issues, when I do, I will gladly share the files with anyone interested. Remember with mastercam you need the Control file, Machine definition file and the post processor file to make it all work.

eatonme!?! seriously? can I call you anything else? please? LOL

Since you have the same machine that I do I would very much appreciate a copy of your machine definition, controller and post files. I am interested in leaning how to work on this.

I suppose I should wait for a private message,,,, or something like that? Not sure if I should post my work email here.

thanks in advance for anything you can share,

Lee

I am currently waiting for a response from Mastercam (X6) for our SLX Prototrak lathe. If I hear back and hopefully I will soon I'll post what they tell me here.

Late to the party....

Can't speak for the lathe, but I have a good working post for the 2 1/2 axis mill.
Prog in mcam as per normal setting depths and depth cuts etc. Mcam outputs as .nc (so it loads in the editor as all coloured and nice to read).
Rename extention .gcd
Load to machine and run.
As the machine is a manual Z, the machine pauses and prompts 'set Z-1.0' (or whatever), so you plunge and lock the quill and press the go and way it runs to the next Z call where it will pause and say 'Check z' (or whatever).
With this post you can make some fancy jobs.
The only thing I gave up on was cutter comp. Prototrak does its own lead in and when using 'machine' (never tried wear), as the machine applied the roll on, prototrak added another roll on of it's own so I gave up.
Perhaps I'll try wear one day...

Anyway, we have a 1630 lathe and it's great - got the dxf converter but never needed it yet.
I would be definately interested in a 'swapsey' :D - lathe mc/control def + post for the prototrak mc/conrtol def + post!
Cheers

Thanks for your response. I too have a prototrak 2-1/2 axis with the SMX control and had no problems using virtually any mill post by opening it with the g-code converter .gcd or .cam file extensions. In fact that was a big contributing factor in choosing the SWI Trak 1630 lathe. Big disappointment when I found so many issues getting a trouble free post for using MasterCam for programming. Well, I'm back to work on it and am getting pretty close. I am working with a guy from MasterCam and I think one more iteration of edits and we'll have it nailed. There are a couple things that I'm not sure we are going to be able to fix like peck drill cycles and tapered threading. Good news is that it's very easy to insert those into a program with prototrak's conversational system. When I feel like the post is a good as it's going to get I will gladly make it available. Thanks...

Bringing up from dead, as I am now lucky enough to try programming one of these lathes with the built in conversational system, which sucks, and is not intuitive at all. Of course I'm used to using Hurcos mill conversational system(don't know about their lathe stuff) and loved it. This Prototrak lathe conversational system bites though. It makes no sense, and doesn't even allow me to spec out my tools appropriately. It adds my nose radius to all turn events that I program, but when I do a cycle turn, it comps correctly but does not make my life easy for programming. Simple face turn(plunging into the face of a part and turning it into a "dish" shape) takes me almost 15 min to get something I think will work.

Podrías enseñarme