Right Angle Head (Aggregate Router) road block

[ETC Don]

I have g code programs, generated by previous engineers, that work on the CNC with an aggregate (RAH) router without an issue. 

I created a g code program with Mastercam that returns an alarm 27 No Axes commanded in G43/G44.  I'll include the text file.

I assumed the problem would be the Machine/ Control definitions and Post combination.  I am able to use two of the three from the working programs, but when I try to use the same machine definition Mastercam returns "Selected machine does not have a valid axis combination". 

It has:  Machine Base

                 Router Table Group

                 Router Head Group

                 Tool Changer Group

Do I need to add the Axes?  I am not sure what is required for the Machine definition file, I believe this one was created specifically for the aggregate router.  I don't know if it was accidentally modified or what.  I also included a .z2g.

Besides this forum, I don't know who else to ask about this.

Thanks

 

EDS 80 SASH GU 1590 RH 45A.txt EDS 80 SASH GU 1590 RH 45A.Z2G

[crazy^millman]

16 minutes ago, ETC Don said:

I have g code programs, generated by previous engineers, that work on the CNC with an aggregate (RAH) router without an issue. 

I created a g code program with Mastercam that returns an alarm 27 No Axes commanded in G43/G44.  I'll include the text file.

I assumed the problem would be the Machine/ Control definitions and Post combination.  I am able to use two of the three from the working programs, but when I try to use the same machine definition Mastercam returns "Selected machine does not have a valid axis combination". 

It has:  Machine Base

                 Router Table Group

                 Router Head Group

                 Tool Changer Group

Do I need to add the Axes?  I am not sure what is required for the Machine definition file, I believe this one was created specifically for the aggregate router.  I don't know if it was accidentally modified or what.  I also included a .z2g.

Besides this forum, I don't know who else to ask about this.

Thanks

 

EDS 80 SASH GU 1590 RH 45A.txt 21.28 kB · 0 downloads EDS 80 SASH GU 1590 RH 45A.Z2G 205.42 kB · 0 downloads

That old of a version using a post created in 2003. That post says you need  to run the old aggregate Chook. Going back that far I cannot remember if that was still required or if adding the aggregate to the MMD was what was needed. No way for me to test.

[ETC Don]

17 hours ago, crazy^millman said:

That post says you need  to run the old aggregate Chook.

When I run aggregat Chook, I get:

Version 9 Aggregate toolpaths can not be edited.

Please select an appropriate machine definition in your machine group properties and re-select the aggregate tools in the source operations if you wish to make changes.

I'm not sure where to go from here.

[JParis]

An aggregate head needs to be defined in the machine def before you can use it.

[ETC Don]

I have a couple machine definition files with all the aggregate specifications.  I just don't know what I am missing.

[ETC Don]

[JParis]

Have you asked your reseller?

I am just wondering if you don't have something that is corrupt..

[ETC Don]

I did ask my reseller, they will be looking into it, but it may be a bit before they get to it.

[ETC Don]

So, the reason (I figured out finally) for the

Alarm 27 NO AXES COMMANDED IN G43/G44

G-code:

N350 G18 G44 H42

was fixed by adding a Y position, Y0.001, after the H42.  Where in the post file would this go?

 

[ETC Don]

In the following g code, when in G18, is it necessary to go to G17 for a Y move and then back to G18?  I wouldn't think so, but I'm looking for other opinions before I comment it out.

N5840 G17 X74.0908 Y-6.
N5850 G18 G44 H42 Y.001
N5860 Z.95
N5870 Y.775
N5880 G01 Y1.3 F25.
N5890 X70.1533 F85.
N5900 G02 X70.0783 Z.875 I0. K-.075
N5910 X70.1533 Z.8 I.075 K0.
N5920 G01 X74.0908
N5930 G02 X74.1658 Z.875 I0. K.075
N5940 X74.0908 Z.95 I-.075 K0.
N5950 (G17) G01 Y1.725 F25.
(N5960 G18 G44 H42)
N5970 X70.1533 F85.
N5980 G02 X70.0783 Z.875 I0. K-.075
N5990 X70.1533 Z.8 I.075 K0.
N6000 G01 X74.0908
N6010 G02 X74.1658 Z.875 I0. K.075
N6020 X74.0908 Z.95 I-.075 K0.
N6030 (G17) G01 Y2.15 F25.
(N6040 G18 G44 H42)
N6050 X70.1533 F85.
N6060 G02 X70.0783 Z.875 I0. K-.075
N6070 X70.1533 Z.8 I.075 K0.
N6080 G01 X74.0908
N6090 G02 X74.1658 Z.875 I0. K.075
N6100 X74.0908 Z.95 I-.075 K0.
N6110 (G17) G01 Y2.575 F25.
(N6120 G18 G44 H42)
N6130 X70.1533 F85.
N6140 G02 X70.0783 Z.875 I0. K-.075
N6150 X70.1533 Z.8 I.075 K0.
N6160 G01 X74.0908
N6170 G02 X74.1658 Z.875 I0. K.075
N6180 X74.0908 Z.95 I-.075 K0.

[ETC Don]

So this becomes a Post question. 

I don't need to change to G17 for any Y moves while in G18.

Where would I look in the post file to change that?

I'm not trying to take the easy way out.  Just the quicker way at this point.  I'm trying to learn post editing enough so I can be helpful on the forum, I'm just not there yet.

[H.tom]

On 8/2/2022 at 11:14 PM, ETC Don said:

So this becomes a Post question. 

I don't need to change to G17 for any Y moves while in G18.

Where would I look in the post file to change that?

I'm not trying to take the easy way out.  Just the quicker way at this point.  I'm trying to learn post editing enough so I can be helpful on the forum, I'm just not there yet.

Look for the following in the post:

   # Start of File and Toolchange Setup
  # --------------------------------------------------------------------------
  pplane_out      #Output Plane G43/G44 and secondary offset when using aggregate (not moulder/not horiz drill)
           if tlplnno$ = 2 | tlplnno$ = 3 |
            tlplnno$ = 5 | tlplnno$ = 6, pbld, n$, *sgplane, *sg43g44, *tlngno2,  yabs, e$   

 

Change "yabs" to "*yabs"

  # --------------------------------------------------------------------------
  pplane_out      #Output Plane G43/G44 and secondary offset when using aggregate (not moulder/not horiz drill)
           if tlplnno$ = 2 | tlplnno$ = 3 |
            tlplnno$ = 5 | tlplnno$ = 6, pbld, n$, *sgplane, *sg43g44, *tlngno2,  *yabs, e$   

[ETC Don]

Thanks.  I'll give that a try and let you know.

[ETC Don]

That took care of the missing Y value, and so slipping back and forth from G18 to G17 doesn't matter, except:

When using the aggragate in the C180 direction, the offset should be H43.

However, in the C0 direction it's H42.

The Post is only using H42.  C180 has a 3 inch bit, where C0 is just over 1 inch.

How do I get it to use the correct offset?