Help with code for Proto Trak AGE 3 controller.

I have a 97 Trak DPM mill with an AGE 3 controller. I am trying to start programing it using my Cad/Cam software made by Vectric. The Vectric software I use on my router table and have used it for 6 years the mill I have always programed using the conversational programing at the head. Vectric wrote me a post processor but it must have a small glitch. I tried to run a small drilling program consisting of 6 holes in .250 5052 Al plate. I drilled through the material in the program by .100" and peck drilled using 2 pecks.

The machine runs to each location requiring a drilled hole hesitates and moves to the next hole location never plunging to drill. I am not used to programing G code but I looked up all the codes and they seem right to me except maybe it is missing the command for a drilling cycle 83. I will post this code and a note from the guy at SWI about what codes the control can take. I am hoping to get this working because I have more parts to make that would take a long time to program at the controller.

The code.

Proto Track Post processor drilling path that did not plunge to drill.

%
:1248
N20G40G80G20G90
N30T1M6
N40G0X0.0000Y0.0000Z0.8000S2500M3
N50G0X0.3000Y1.9000Z0.2000
N60G1Z-0.1750F3.0
N70G0Z0.0000
N80G1Z-0.3500F3.0
N90G0Z0.2000
N100G0Y3.8500
N110G1Z-0.1750F3.0
N120G0Z0.0000
N130G1Z-0.3500F3.0
N140G0Z0.2000
N150G0Y5.7900
N160G1Z-0.1750F3.0
N170G0Z0.0000
N180G1Z-0.3500F3.0
N190G0Z0.2000
N200G0Y7.7250
N210G1Z-0.1750F3.0
N220G0Z0.0000
N230G1Z-0.3500F3.0
N240G0Z0.2000
N250G0X6.7845Y0.5000
N260G1Z-0.1750F3.0
N270G0Z0.0000
N280G1Z-0.3500F3.0
N290G0Z0.2000
N300G0X5.5345Y0.5000
N310G1Z-0.1750F3.0
N320G0Z0.0000
N330G1Z-0.3500F3.0
N340G0Z0.2000
N350G0Z0.8000
N360G0X0.0000Y0.0000
N370M2
%

The note from Joseph @ SWI

The list of accepted G code are as follows

G0

G1

G2 & 3

G20 & 21

G40, 41 & 42

G73 Peck drilling cycle

G80 Drilling cycle cancel

G81 Drilling cycle, spot boring

G82 Drilling cycle, counter boring

G83 Peck drilling cycle

G85 Boring cycle

G89 Boring cycle, dwell at bottom

G90 & 91



M Codes

M0, 2, 5, 6, 7, 8, 9, 12 & 20. All other M codes are simply ignored.

Thank you for any help you can offer.

Mike

145 views and no ideas or is it too easy I should not be asking? I run a small business and machine my products I am not a job shop guy with a lot of experience. I try hard and figure out a process then reproduce those parts in house I don't have near the knowledge most of you guys have I try not to ask dumb questions but maybe this is a dumb question and I don't know enough to realize it. I could program this very easily for my router table but my router spindle is not designed for drilling aluminum the best tool for the job is the mill.

I am considering getting a different control for this machine that would make programing it simple like the router. The newer control that Trak makes is $9000 + I am not sure spending that much on this old machine is worth it.

Mike

I think you might be struggling for a response on this because most people program at the control on these machines ,as I do .Sorry that I can't be more help.

We had one of those at work for a long time, we just traded it in on a new one. Ours wasn't worth upgrading with the new control.

Is the Z coming down to the clearance plane? It's been awhile since I've run one of those, but can't you switch between AGE 2 and 3 and run it as a 2 axis or 3 axis machine?

It looks like on your program you won't need the G83, because it's being output point to point.

Do NC programs need to be run as .GCD, like on the newer machines?

amm1060 said:

We had one of those at work for a long time, we just traded it in on a new one. Ours wasn't worth upgrading with the new control.

Is the Z coming down to the clearance plane? (Yes) It's been awhile since I've run one of those, but can't you switch between AGE 2 and 3 and run it as a 2 axis or 3 axis machine? (Yes)

It looks like on your program you won't need the G83, because it's being output point to point. (that is what I thought but it doesn't work)

Do NC programs need to be run as .GCD, like on the newer machines?

Click to expand...

(In the programing manual it says it must be a file named with a number example 1234 followed by dot CAM or dot MX3 example 1234.CAM or 1234.MX3. All of the programs made at the controller have the MX3 and anything you import from CAM must be the number with .CAM at the end. That is the only info I have.)

I could easily program this simple drilling path at the head but I have more complex parts to make and I am just trying to get this thing to work with a post processor. Thank you for the replies.

I have sent an email to Vectric and SWI but I have not heard back from them yet.

.CAM sounds right. The .GCD is for the newer SMX control. I wish we still had the old Prototrak so I could test that program out and find out what the deal is. I don't think we ever ran a CAM program on ours, we just started running them on our SMX mills. On those we just use a generic Hurco post with no problems.

Is there a dry run function that locks out Z moves that could be turned on?

Joseph at SWI is pretty good to deal with. I just talked to him last week on some software issues. It's best to get him on the phone instead of trying to go through email.

prototrak

1) you need all the manuals for a Prototrak AGE3.
XYZ Machine Tools Reference - Manuals

has some manuals but you may have to buy the cadcam manual from SWI web site as older machines are not fully listed. manual 20260 the cadcam manual is listed on attached parts list
.
2) some machine require the X and Y and Z coordinate on each line even if they do not change. If you just list G1 Z-1. F1. it probably will not work no X and Y on the line too.
I am reading attached pages and peck drilling is G83 or G73, you have to list peck amount and retract amount too.
G80 is canned drilling cycle cancel
.
3) writing post processors is often trail and error. I would write simple program test G0 move by itself, the G1, then G2 and so on only one at a time until you got everything Gcode working

gundog said:

I have a 97 Trak DPM mill with an AGE 3 controller. I am trying to start programing it using my Cad/Cam software made by Vectric. The Vectric software I use on my router table and have used it for 6 years the mill I have always programed using the conversational programing at the head. Vectric wrote me a post processor but it must have a small glitch. I tried to run a small drilling program consisting of 6 holes in .250 5052 Al plate. I drilled through the material in the program by .100" and peck drilled using 2 pecks.

The machine runs to each location requiring a drilled hole hesitates and moves to the next hole location never plunging to drill. I am not used to programing G code but I looked up all the codes and they seem right to me except maybe it is missing the command for a drilling cycle 83. I will post this code and a note from the guy at SWI about what codes the control can take. I am hoping to get this working because I have more parts to make that would take a long time to program at the controller.

The code.

Proto Track Post processor drilling path that did not plunge to drill.

%
:1248
N20G40G80G20G90
N30T1M6
N40G0X0.0000Y0.0000Z0.8000S2500M3
N50G0X0.3000Y1.9000Z0.2000
N60G1Z-0.1750F3.0
N70G0Z0.0000
N80G1Z-0.3500F3.0
N90G0Z0.2000
N100G0Y3.8500
N110G1Z-0.1750F3.0
N120G0Z0.0000
N130G1Z-0.3500F3.0
N140G0Z0.2000
N150G0Y5.7900
N160G1Z-0.1750F3.0
N170G0Z0.0000
N180G1Z-0.3500F3.0
N190G0Z0.2000
N200G0Y7.7250
N210G1Z-0.1750F3.0
N220G0Z0.0000
N230G1Z-0.3500F3.0
N240G0Z0.2000
N250G0X6.7845Y0.5000
N260G1Z-0.1750F3.0
N270G0Z0.0000
N280G1Z-0.3500F3.0
N290G0Z0.2000
N300G0X5.5345Y0.5000
N310G1Z-0.1750F3.0
N320G0Z0.0000
N330G1Z-0.3500F3.0
N340G0Z0.2000
N350G0Z0.8000
N360G0X0.0000Y0.0000
N370M2
%

The note from Joseph @ SWI

The list of accepted G code are as follows

G0

G1

G2 & 3

G20 & 21

G40, 41 & 42

G73 Peck drilling cycle

G80 Drilling cycle cancel

G81 Drilling cycle, spot boring

G82 Drilling cycle, counter boring

G83 Peck drilling cycle

G85 Boring cycle

G89 Boring cycle, dwell at bottom

G90 & 91



M Codes

M0, 2, 5, 6, 7, 8, 9, 12 & 20. All other M codes are simply ignored.

Thank you for any help you can offer.

Mike

Click to expand...

This has been a learning experience and I think that is good but I wished it had been quicker. The post processor Vectric wrote me did not work when the mill was in the AGE 3 mode with .CAM as the format. I was having a conversation with Joesph @ SWI when it clicked he told me what I was trying to do required a DNC key which I have he then told me the files needed to have the part number followed by .DNC to get the machine to work in full 3D mode apparently in AGE 3 mode it only actually works in 2.5D meaning it can do X&Y at the same time but Z can not move at the same time it pauses to move in Z then again will move in X&Y.

The DNC key is an upgrade and it unlocks additional memory as well as allows a CAM program to run the machine in full 3D. The programs were written in a way the controller did not like in the AGE 3 mode but work fine in DNC mode. I had to rename the files in .DNC after the part number to make this work. You must also open the machine in the DNC mode which works a little different than it does in the MX3 mode or CAM mode, this little part was throwing me off. When you choose a part program in MX3 or Cam mode you choose program in/out and those files are shown to choose from but the DNC programs can't be chosen in this mode, this is the part that was throwing me off. You need to choose DNC mode and choose run this scared me at first I was afraid choosing run would cause motion on the machine but when in DNC mode after choosing run it goes to another menu where you can choose floppy drive or RS 232. This allowed me to then choose the files renamed with .DNC and the files worked fine even the drilling program I posted in this thread earlier ran just fine in this mode.

I have now been able to design parts and cut them using my Cad/Cam program and it actually works this is a huge milestone for me. I am posting this in case it helps someone else going through this. They finally sent me the CAD/Cam, DNC RS 232 interface manual today and I was able to sort this out with the info they had given me. This is not real intuitive without the proper documentation. Hopefully it may help someone out in the future if they do a search and can figure out my rambling.

Mike

Hi,

I know this thread is now 6 years old but it explains a lot and I am looking for a DNC key to enable me to do the same type of programs

If anybody has one available please message me

Thanks
Marc