Prototrak SMX programming

cj133 · Nov 29, 2017

Hi all,

Very new to this but want to learn.
I'm working with a Prototrak SMX FHM 7 and want to use cad cam software with it.

Right now, it seems I have two options. To load G code into the machine as a .CAM file and have it convert it to it's own code, or to load a .GCD file and run raw G code. Is this correct?

Currently the guy I work with takes autocad files from me and loads them into Prototrak's software and then does what he needs to from there. I'd like to take it a step further than that.

I saw in the book it mentions running straight G code for complicated programs as well as if you want to use it as a full 3 axis machine but they don't really go into much detail.

I've got a lot of learning to do, but need someone to point me in the right direction if possible. :cheers:

Stihl290 · Nov 29, 2017

cj133 said:
Right now, it seems I have two options. To load G code into the machine as a .CAM file and have it convert it to it's own code, or to load a .GCD file and run raw G code. Is this correct?

The latter half of this statement is correct. Generate your program and tool path with CAM software and save it as .GCD file. Open up the file, setup the part/tools/work offset ,etc. and it should be all good to go. Just make sure you have the right post.

As far as the .CAM file, it sounds right but I cannot vouch for it.

NX - CAM · Nov 30, 2017

I am learning the ProtoTRAK SMX too.
Do you have the Optional option for SMX : DXF and Parasolid ?
You have these options :
- programming on machine display (with conversational SMX, named ...events)
- programming off line with a simple G code editor or SMX software (offline SMX software)
- using CAM and convert to G code, with an "issue" here and that is that the CAM software may not have the SMX Postprocesor and it may generate G codes not recognised by SMX. For the entire list, SMX recognize only a few G,M codes.
If you have the option of importing DXF and/or Parasolid that your life is much easier on creating the tool path.
Hope this help.

cj133 said:
Hi all,

Very new to this but want to learn.
I'm working with a Prototrak SMX FHM 7 and want to use cad cam software with it.

Right now, it seems I have two options. To load G code into the machine as a .CAM file and have it convert it to it's own code, or to load a .GCD file and run raw G code. Is this correct?

Currently the guy I work with takes autocad files from me and loads them into Prototrak's software and then does what he needs to from there. I'd like to take it a step further than that.

I saw in the book it mentions running straight G code for complicated programs as well as if you want to use it as a full 3 axis machine but they don't really go into much detail.

I've got a lot of learning to do, but need someone to point me in the right direction if possible.

cj133 · Nov 30, 2017

NX - CAM said:
I am learning the ProtoTRAK SMX too.
Do you have the Optional option for SMX : DXF and Parasolid ?
You have these options :
- programming on machine display (with conversational SMX, named ...events)
- programming off line with a simple G code editor or SMX software (offline SMX software)
- using CAM and convert to G code, with an "issue" here and that is that the CAM software may not have the SMX Postprocesor and it may generate G codes not recognised by SMX. For the entire list, SMX recognize only a few G,M codes.
If you have the option of importing DXF and/or Parasolid that your life is much easier on creating the tool path.
Hope this help.

We do have the DXF converter and it's how we're currently using the machine.
But to me, it seems like an awfully awkward and archaic way of doing things. I was hoping running G code from a CAM program would be faster but it's sounding like that's not the case.

How does the Parasolid converter work? Will it gain us anything over the DXF converter if I get the proper CAM software to work with it?

I had looked into getting Prototrak's offline software but I couldn't imagine spending what they want for it.

NX - CAM · Dec 2, 2017

Parasolid, from this point of view, is the same : archaic !
Compared to DXF, here you can select the depth !
CAM software is ok, depending of the parts complexity.
But again, the postprocesor which create the G-code in CAM , need to be for ProtoTRAK SMX.
Otherwise you will need to debug/delete/replace the G codes generated by CAM post procesor and not recognized by SMX.
Try a simple part in CAM, see the G-code , and run it on SMX !

cj133 said:
We do have the DXF converter and it's how we're currently using the machine.
But to me, it seems like an awfully awkward and archaic way of doing things. I was hoping running G code from a CAM program would be faster but it's sounding like that's not the case.

How does the Parasolid converter work? Will it gain us anything over the DXF converter if I get the proper CAM software to work with it?

I had looked into getting Prototrak's offline software but I couldn't imagine spending what they want for it.

swarf_rat · Dec 3, 2017

My experience is not with the SMX control, but the SLX - same control but for a lathe. You can generate a G-Code file for it, but the post processor has to be set up properly to only produce those codes the control will interpret - generally Fanuc 6 level. The codes it accepts are listed in the Prototrak manual.

One problem with this method is the control will convert the code to its own PT4 file (at least on the lathe, and I believe the mill is the same). You will end up with very verbose code, since it cannot translate the g-code into Prototrak cycles, making it very hard to make even small edits at the control if needed. I found this made for often cumbersome operation - any change had to go back through the whole process.

To solve that problem, I wrote my own post processor (for OneCNC) that produces something like the native .PT4 format. It is not complicated but is also not documented by Prototrak so I had to reverse engineer it. Some CAM post processors would be capable of producing an executable .PT4 file, but OneCNC does not have sufficient flexibility in the post processor, so I wrote a PC program that post processes the post process file, fixing the problems. My work flow is now OneCNC->CAM out->home grown post processor->transfer to machine. One step (but just a double click) from the way any CNC should work. The resulting program comes into the Prototrak as a native .PT4 file, preserves all cycles, and is easily editable at the control.

I've been told not everyone has the skill to do this - but if you have any computer programming experience it is relatively easy. The .PT4 file is just a list of text records, and not difficult to understand. All of the programming is simple text manipulation.

cj133 · Jan 8, 2018

Have been using Fusion 360 with a G code post processor with good success so far.
It is true I cannot modify anything on the machine, but I can go back to the PC and do what I need to.

So far, the biggest issue has been working with the tool table on the SMX. The procedure here, has been to clear the tool table every time and start from scratch with each project. I'm thinking it's time to change this if possible because it's extremely time consuming.

I see in the book I can set up tools using a reference tool and the table for height. It appears the machine looses this anytime the computer loses power, or, anytime a Prototrak program is loaded. My thoughts are to make a program on the machine with nothing other than the tool table. This way, I can load the table if need be and then load my G code program and set my ABS points.

Has anyone tried this on the Prototrak SMX? I don't see any reason it wouldn't work but I haven't tried yet. I'd like to have our most common 10-20 tools all set up and ready to go for every program. Best I can tell, loading G code programs doesn't appear to effect the tool table.

TDegenhart · Jan 8, 2018

I purchased the Prototrak DXF converter software and the offline programming software with dongle a couple of years ago but other installing and setting it up, I haven't used it. The stuff I run on the mill are simple enough to program at the machine. If you are interested in purchasing, contact me with a PM.

Tom

MeanMachine1980 · Jan 5, 2020

cj133 said:
Have been using Fusion 360 with a G code post processor with good success so far.
It is true I cannot modify anything on the machine, but I can go back to the PC and do what I need to.

So far, the biggest issue has been working with the tool table on the SMX. The procedure here, has been to clear the tool table every time and start from scratch with each project. I'm thinking it's time to change this if possible because it's extremely time consuming.

I see in the book I can set up tools using a reference tool and the table for height. It appears the machine looses this anytime the computer loses power, or, anytime a Prototrak program is loaded. My thoughts are to make a program on the machine with nothing other than the tool table. This way, I can load the table if need be and then load my G code program and set my ABS points.

Has anyone tried this on the Prototrak SMX? I don't see any reason it wouldn't work but I haven't tried yet. I'd like to have our most common 10-20 tools all set up and ready to go for every program. Best I can tell, loading G code programs doesn't appear to effect the tool table.

Hello

Did you ever get this to work on your smx controller?

I have the same exact gripe. Whenever I load a GCD file from my cam I have to go into the tool table and set the tool reference. And also renumber the tools to match up to the cam program if they were different.
Thanks

cj133 · Jan 7, 2020

MeanMachine1980 said:
Hello

Did you ever get this to work on your smx controller?

I have the same exact gripe. Whenever I load a GCD file from my cam I have to go into the tool table and set the tool reference. And also renumber the tools to match up to the cam program if they were different.
Thanks

Yep,
Pretty much just set your tool table up and leave it alone.

I believe every time you load a program it's going to say the reference height isn't set anymore. It only matters if you need to set a tool up or change one. You can just load the program, run it and ignore the "make sure your tools are right" error that pops up.

What I do on ours is I have a tool on the side that's never used. I use that with a little electric light up height setter on the table. If I need to change a tool I quickly set my reference height using that tool that's never used and than I can swap tools without changing the others. The tool you use for reference doesn't need to be in the list, just keep it on the side.

bmoss147 · Jan 14, 2022

yea i was thinking of purchasing this do you still have it

cj133 · Jan 14, 2022

bmoss147 said:
yea i was thinking of purchasing this do you still have it

Yep, it's one of our most used machines.
It's not perfect, but it makes money.

rancid990 · Jul 31, 2023

swarf_rat said:
My experience is not with the SMX control, but the SLX - same control but for a lathe. You can generate a G-Code file for it, but the post processor has to be set up properly to only produce those codes the control will interpret - generally Fanuc 6 level. The codes it accepts are listed in the Prototrak manual.

One problem with this method is the control will convert the code to its own PT4 file (at least on the lathe, and I believe the mill is the same). You will end up with very verbose code, since it cannot translate the g-code into Prototrak cycles, making it very hard to make even small edits at the control if needed. I found this made for often cumbersome operation - any change had to go back through the whole process.

To solve that problem, I wrote my own post processor (for OneCNC) that produces something like the native .PT4 format. It is not complicated but is also not documented by Prototrak so I had to reverse engineer it. Some CAM post processors would be capable of producing an executable .PT4 file, but OneCNC does not have sufficient flexibility in the post processor, so I wrote a PC program that post processes the post process file, fixing the problems. My work flow is now OneCNC->CAM out->home grown post processor->transfer to machine. One step (but just a double click) from the way any CNC should work. The resulting program comes into the Prototrak as a native .PT4 file, preserves all cycles, and is easily editable at the control.

I've been told not everyone has the skill to do this - but if you have any computer programming experience it is relatively easy. The .PT4 file is just a list of text records, and not difficult to understand. All of the programming is simple text manipulation.

Hi swarf_rat!

We have a ProtoTRAK SM Bed Mill at work. That doesn't have the "CAM File Out Converter" option, so no GCODE for us. I've emailed SWI for a quote on a license key for it. But I feel pretty uneasy spending hundreds of dollars on license for a 22 year old discontinued bit of equipment.

Would you be willing to share your .pt4 processor? If not I was planning on attempting to write one myself. It would probably be a good learning exercise for my programming skills haha!

Search

Largest Manufacturing Technology Community on the Web

Search

Prototrak SMX programming

cj133

Aluminum

Stihl290

Aluminum

NX - CAM

Plastic

cj133

Aluminum

NX - CAM

Plastic

swarf_rat

Titanium

cj133

Aluminum

TDegenhart

Diamond

MeanMachine1980

Aluminum

cj133

Aluminum

bmoss147

Plastic

cj133

Aluminum

rancid990

Plastic

Similar threads