Prototrak turn/lathe post processor

[Pillnoob]

  I think it would be nice if you guys could offer a post processor for the prototrak lathe. After some fumbling around this weekend I was able to "piece" together a program good enough to run but a more streamline process would be ideal.
 
  The prototrak lathe will not convert an "R" value for G2 or G3 so It will have to post process with I/K arc centers (incremental center point, of the diameter)  or point to point moves like the " heidenhain turning" post processor. This shouldn't be very hard to make and I would be willing to offer my time and machine up for Beta testing purposes.

For starters the machine recognizes G97 as RPM mode and G98 IPM, SPM and IPR are enable on the machine only if the advance features option is enabled. G96 is for surface speed and G99 is per revolution feed.

Here is a sample attached program posted as heidenhain turning

O1510
N10 G94 (Delete out)
N15 G26 S6000 (Delete out)
N20 G14
N25 M09
N30 T101 (make this post as actual tool number not plus 100)
N35 M08
N40 G95 (not recognized delete out)
N45 G96 S500 M03 (use G97)
N50 G26 S3000 (use IPM g98 or G99 for F value)
N55 G00 X3.05 Z0.0266
N60 G00 X0.5085
N65 G01 X0.3546 F0. (change to make it hold the actual federate programed in the CAM system instead of outputting to zero)
N70 X0.2414 Z-0.03
N75 X0.2684 Z-0.0331
N80 X0.2708 Z-0.0334
N85 X0.3172 Z-0.0399
N90 X0.3195 Z-0.0402

The control will recognize basic "canned cycles" but does not like G54, G18/G19, G26 and G50.

[HughesTooling]

Can you try the Fanuc post try setting the type to A, B or C. There was a problem with IK output not sure if that's fixed but I've fixed my post so could upload here if the code looks close. I think type B might be closer to what you want.

Mark

[Pillnoob]

We will give that a try can you enlighten me as to what the posting "type" does inside the program?

Thanks.

[HughesTooling]

Type A, B and C will give you different codes for setting max RPM, surface speed and feed per min or feed per rev. I just looked at the post supplied with Fusion and it still has a bug\typo where it scales the I and K wrong, it's set to scale both to diameter but they should both be unscaled. Give it a try on something simple, if there's an IK error it's an easy fix.

@xander.luciano I've reported this problem and tagged in support several times and it never gets a response. Can you take a look.

In the generic post both I and K use xFormat, xFormat scales by 2.

var kOutput = createReferenceVariable({prefix:"K"}, xFormat);
var iOutput = createReferenceVariable({prefix:"I"}, xFormat); // no scaling

To get IK to work on my control I changed to use zFomat for both.

var kOutput = createReferenceVariable({prefix:"K"}, zFormat);
var iOutput = createReferenceVariable({prefix:"I"}, zFormat); // no scaling

Mark

[xander.luciano]

@HughesTooling

Hmm, I'm not too familiar with lathes and their posts myself (I run mills), but I and J should represent a vector distance from the start point to the center point.

Just looked at the post on my end and I do see that xFormat is using a scale of 2 and the I/K outputs are both using the format. Wouldn't you want the I output to be scaled 2 if the x is scaled by 2? Though I don't think the Z output would be scaled. Either way the comment says no scaling but it's being scaled so something doesn't seem right here. The radius output is correct though:

// circular output
var kOutput = createReferenceVariable({prefix:"K"}, xFormat);
var iOutput = createReferenceVariable({prefix:"I"}, xFormat); // no scaling

var g92ROutput = createVariable({prefix:"R"}, zFormat); // no scaling

I'll definitely bring this up with the posts guys though, I'm surprised nothing's been said about it before. 

Thanks for catching this!

Best,
-Xander Luciano

[Pillnoob]

Be very careful with this, I had did a test run on this today posted as the HAAS with I/K values and it worked just fine for me today. The I and K values should be an incremental move form the arc start point no matter if an I or a K. The X value is almost defined as diameter in any of the CNC lathes today unless a radial option is selected.

[xander.luciano]

Thanks! Just wanna make sure I'm getting everything correct here.

> "The X value is almost defined as diameter"

The haas-turning.cps post doesn't use diameter mode though? Unless I'm understanding something wrong here (which I might be, I really only work with mills). Here's the formatting code:

var spatialFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true});
var xFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true, scale:2}); // diameter mode
var yFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true});
var zFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true});
var rFormat = createFormat({decimals:(unit == MM ? 3 : 4), forceDecimal:true}); // radius

// circular output
var iOutput = createReferenceVariable({prefix:"I", force:true}, spatialFormat);
var jOutput = createReferenceVariable({prefix:"J", force:true}, spatialFormat);
var kOutput = createReferenceVariable({prefix:"K", force:true}, spatialFormat);

var g92IOutput = createVariable({prefix:"I"}, zFormat); // no scaling

The xFormat uses scale:2 and says diameter mode, spatialFormat does not use scale 2, and therefore I would assume means that the IJK values are not scaled by 2. Correct me if I'm wrong here.

Maybe I'll just program a few test parts and see what code gets posted. At minimum I can understand the X axis being scaled or not scaled, but I would the Z axis to not be scaled. 

Thanks for the info,

Xander Luciano

[Pillnoob]

    Sorry but I am not the best at understanding the post processor language but after some more testing it did output to the diameter in X for me after another try with the HAAS post processor. You are correct today almost all CNC lathes use a diameter value for X that's not only how they are programed but also how they are picked up/set up. From my experience I, J and K values are always incremental.  The Z axis is never scaled if you need to move down the part 2 inches that's what would be programmed. If you need any help with the post on this I would run what ever programs through my prototrak lathe for beta testing.

[HughesTooling]

Although the X is in diameter mode the incremental distance to IK and is just the distance no scaling. If you look at the Haas example the X is scaled but IJK all use spatialFormat so no scaling and that's correct.

Just looked in my manual and it says I words are programed as radius moves. I have done the zFormat mod on my post, one for a Fanuc 21i and one for a Chinese clone and they both work also modified the post for 2 or 3 people on the forum.

Mark

[HughesTooling]

---

@xander.luciano wrote:

@HughesTooling

I'll definitely bring this up with the posts guys though, I'm surprised nothing's been said about it before. 

Thanks for catching this!

Best,
-Xander Luciano

---

The default is to use R so a lot of people will not notice. When I first found the problem I was too busy to investigate and to get the job done used R, it was only when someone else brought it up on the form that I figured out what was wrong. I think it's just a typo because you'd never scale the Z\K and it even says No scaling on the iOutput line.

Mark

[xander.luciano]

Hey Mark!

I had one of our post guys make that change, so should be corrected in the post library in the next version! He also removed the G17 output during canned cycles from another user report on the forums.

Thanks once again!
Xander Luciano

[Pillnoob]

When do you think that post will come out? Also are you guys planning on a specific prototrak lathe post?

[xander.luciano]

I'm not sure how often our posts library is updated and pushed, but I would probably say a week or 2? I could get you the updated version earlier if you need it though.

As far as a prototrak lathe post, that I cannot say for certain. Usually we defer to the forums for post modifications. Often times our users will have more experience with less common controllers. If you have trouble getting a post that works for you, that's where users like @HughesTooling tooling and myself come in. Just post any issue you are running into and what codes are wrong, or what needs to be changed and we'll get things updated for you!

Hope that helps!
-Xander Luciano

[HughesTooling]

@Pillnoob It looks like the Fanuc type A is close to what you want. I have a test design in Fusion that's an easy test for G02/03 setup, see attached file.

.

Here's the code. This is after fixing the IK output, one thing to check is if the I or K move is zero they are not output. Removing the G54 is no problem, my controls allow G54 not sure if that's all fanuc lath controls. What code do you need for setting the max spindle speed, is G50 correct?

%
O0001
N10 G98 G18
N11 G21
N12 G50 S6000 (ONLY HERE FOR SAFETY SET TO MAX FOR JOB
N13 G28 U0.

(PROFILE1)
N14 T0303
(55 DCMT)
N15 G54  
N16 M8
N17 G98
N18 G50 S5000
N19 G96 S150 M3
N20 G0 X48. Z5.
N21 G0 Z2.
N22 X47.074
N23 G1 X-0.8 F0.5
N24 Z0. F0.3
N25 X9.2 F0.125
N26 G18 G3 X20. Z-5.4 K-5.4
N27 G1 Z-10.4
N28 G2 X29.2 Z-15. I4.6  (K ZERO NOT OUTPUT
N29 G1 X39.2
N30 X43.2 F0.5
N31 G0 X48.
N32 Z5.

N33 M9
N34 G28 U0. W0.
N35 M30

Mark

[HughesTooling]

Picture shows the code for Type A and B, A is Standard G Code. Notice G17/18/19 and G53/54 are not listed

Mark

[Anonymous]

http://www.southwesternindustries.com/media/manuals/24494_manual.pdf

Section 12.12 has alot of info on posting to Trak lathe

[Pillnoob]

On my prototrak the max spindle rpm clamp is actually setup when you first start the machine up. During my testing I was able to output my I and K values just fine so I'm not sure if I have a newer post or what is going on? Everything in the program appears to be acceptable for the prototrak minus the G54.

[Anonymous]

Tool offsets, modifiers, and home positions are defined within the Prototrak control and are ignored through G-Code.

[Pillnoob]

With the expection of tool comp (G40, G41, G42)

[HughesTooling]

---

@Pillnoob wrote:
During my testing I was able to output my I and K values just fine so I'm not sure if I have a newer post or what is going on? Everything in the program appears to be acceptable for the prototrak minus the G54.

---

You say your test was OK with the IK output, were the arc sizes correct or did it just run. The reason I ask is with I and K scaled by 2 in the standard Fanuc post it would probably run but the acrs would be the wrong size.

Here's a post to try. I've made the change to no scaling for IK output, removed the work offset and made the default to output IK not R. Is the line G50 S1500 correct for your control?

Mark

Test the post carefully and I'd better add this 

The accompanying advice and or non-standard post processor is provided as-is and without warranty of any kind, and usage is at the user’s own risk.

Do not put custom posts in the generic posts folder. Use the personal folder. or another location.

Fusion 360 CAM Personal Posts Folder Locations

_______________________________________________________________________________

Microsoft Windows:
%appdata%\Autodesk\Fusion 360 CAM\Posts

Mac / Apple / OSX:
/Users/<user id>/Autodesk/Fusion 360 CAM/Posts