G68.2 G43.4 & G53.1

[So not a Guru]

Can these be used together?

We are having an odd issue with our head-head router. Our post is setup to drill like this:

G56 G17 G90
G90 G43 H39
G00 A-18.435 C0. X3.75 Y18.3259 Z15.0829 M03 S3500
G49
G68.2 X0. Y0. Z0. I180. J18.435 K0.
G53.1
G43 H39
G94
G98 G81 Z15.2689 R17.104 F50.
X-43.25
G80
G49
G69

Trouble is that when the drill retracts from the hole it does not follow the same path it entered with! In a honeycomb panel this creates slots instead of holes, I would imagine it would create broken drills in any material of substance. It has been my understanding that the purpose of G53.1 is to rotate the primary & secondary axes perpendicular to the tilted plane triplet from the G68.2 call. The machines behavior would suggest that I am mistaken.

So I contacted the machine mfg (who are our post reps for the Postability post for some reason) to see if they had a solution. They replied that the above code should be modified with G43.4, instead of G43, because the TCP makes the axes move at the same accel & decel rates for multi-axis moves, and that the G53.1 should be removed thus:

G56 G17 G90
G90 G43 H39
G00 A-18.435 C0. X3.75 Y18.3259 Z15.0829 M03 S3500
G49
G68.2 X0. Y0. Z0. I180. J18.435 K0.
G43.4 H39
G94
G98 G81 Z15.2689 R17.104 F50.
X-43.25
G80
G49
G69

I'm concerned that without the G53.1 the head will move strictly in the Z-axis.

That's why I'm wanting to know if G68.2, G53.1 & G43.4 will play nicely with each other.

[austin noah]

I don't think you should use G43.4 with G68.2.  I think you problem with the first code is that you need to call up X and Y again after the G53.1 when you are in your tilted working plane before you do your drill cycle.

[crazy^millman]

They have not setup the parameters on the machine correctly to support G68.2. They need to get a hold of Marty in Los Angles who works for Fanuc and he can walk them through the correct way to configure the machine to work like it should. I have never used G68.2 and G43.4 like that and curious will that even run on the machine.

There are different parameters to change the behavior of machine when drilling. Have them get a hold of Tim Scott at Postability to help them sort out the different parameters issues.

[huskermcdoogle]

The standard way would be using G43 with G68.2 like you did in the original sample. 

Does the head change angle when you call out G53.1 in your case?

[So not a Guru]

1 hour ago, huskermcdoogle said:

The standard way would be using G43 with G68.2 like you did in the original sample. 

Does the head change angle when you call out G53.1 in your case?

No it doesn't change angle. Neither rotary axis move, it's just that the XYZ axes don't follow the G53.1 rules when retracting out of the holes.

[huskermcdoogle]

Have you tried using G68.3?  You position the rotary axes and call this then you can shift and rotate the coordinate frame around the new spindle axis, G68.3 X Y Z R.  I used to use this if I was hand coding a single hole and wanted to add pecking at the machine at an odd angle.  I wonder if it does the same side shift thing.

[crazy^millman]

32 minutes ago, So not a Guru said:

No it doesn't change angle. Neither rotary axis move, it's just that the XYZ axes don't follow the G53.1 rules when retracting out of the holes.

Which screams parameter issues.

[So not a Guru]

1 hour ago, crazy^millman said:

Which screams parameter issues.

Yeah, that's kind of what I've been thinking too. I haven't heard back from the machine mfg yet, but I'm going to  push for them to get some more info from Fanuc on this.

[cncappsjames]

The usual program format i see is as follows;

G54 A...C...

G68.2 X0Y0Z0I...J...K...

G53.1

X... Y...

G43H...Z...

so on and so forth

G49

G69

...

Your code seems sketchy to me. In order for the functions to work in a predictable manner, some rules need to be followed. 

Activate the work offset with your tilt and rotary angles only. Activate TWP. Activate spindle direction control. Move your X an Y linear axes. Activate tool length offset. 

Do some machining.

Cancel tool length offset.

Cancel TWP.

 

If doing 4/5-Axis cutting then I do as follows;

G54 A...C...

G68.2 X0Y0Z0I...J...K...

G53.1

X... Y...

G69

G43.4H...Z...

so on and so forth

G49

Basically I'll use TWP to preposition, cancel it then activate TCP.  You don't have to do that, I just like to for safety's sake. It's an extra step, sure, but I prefer safety and predictably over speed.

 

JM2CFWIW 

[So not a Guru]

7 hours ago, cncappsjames said:

Your code seems sketchy to me. In order for the functions to work in a predictable manner, some rules need to be followed. 

Activate the work offset with your tilt and rotary angles only. Activate TWP. Activate spindle direction control. Move your X an Y linear axes. Activate tool length offset. 

Do some machining.

Cancel tool length offset.

Cancel TWP.

So I should modify my post (or have Postability do it for us) to output this:

G56 G17 G90
G90 G43 H39
G00 A-18.435 C0. M03 S3500
G49
G68.2 X0. Y0. Z0. I180. J18.435 K0.
G53.1

X3.75 Y18.3259
G43 H39 Z15.0829
G94
G98 G81 Z15.2689 R17.104 F50.
X-43.25
G80
G49
G69

 

[cncappsjames]

G56 G17 G90 G00 A-18.435 C0. M03 S3500
G68.2 X0. Y0. Z0. I180. J18.435 K0.
G53.1

X3.75 Y18.3259
G43 H39 Z15.0829
G94
G98 G81 Z15.2689 R17.104 F50.
X-43.25
G80
G49

 

This is how I would do it.

[crazy^millman]

23 hours ago, So not a Guru said:

So I should modify my post (or have Postability do it for us) to output this:

G56 G17 G90
G90 G43 H39
G00 A-18.435 C0. M03 S3500
G49
G68.2 X0. Y0. Z0. I180. J18.435 K0.
G53.1

X3.75 Y18.3259
G43 H39 Z15.0829
G94
G98 G81 Z15.2689 R17.104 F50.
X-43.25
G80
G49
G69

 

Postability can do that they have made several posts like this for customers we have done projects for. This format comes down to how the builder configured the parameters. Some builders configure them to not requires the DWO or TCP to be mapped from home position. Others need something to map with and by using the G68.2 to positionso  the G43.4 then not have a problem. On smaller machines where the rapids are so fast people don’t care if the machine has to make extra moves to do 5 Axis work. On your machine I would push the builder to not require that and allow you the standard G43.4 and if needed the mapped start point to a point near where you are working to run. The trick will be the process doing several 5 Axis toolpaths with the same tool and getting he correct format out of the post. You normally will not want G49 at the end of each operation out of Mastercam when doing G43.4 operations with the same tool. Again depending on the parameters each machine with Fanuc controls do things odd. A correctly configured machine should allow you to use G68.2 mapped to a different T-C Plane relative to the main WCS.
 

Problem is a lot builders don’t really grasp how to correctly implement it. With Siemens controls almost every builder knows how to configure the control to map CYCLE800 correctly so as a programmer we have freedom to put the T-C plane where ever we want on our part and with a post configured to map it correctly it is a nice process almost anyone running the program can follow. We should have the same ability with all Fanuc machines using G68.2 and G43.4, but because Fanuc for whatever reason has not imbedded it’s people into the machine builders like they should it is a mess and gives Fanuc a black eye. James works with a builder who early on got it and stuck with a good way to go about it, but I don’t like having to always use G68.2 to get G43.3 to do what it should. We should be able to program G43.3 and have any machine run our program without having or needing extra code to run it. That is really what you are fighting here is a lack of overall understanding and implementation from the control supplier to the machine builder.

As we transition into the 4.0 process or digital twin people pushing the sales keep using we need more predictable processes out of the box that work, Matsurra in my opinion is one of a few builders that has gotten it for a long time, Doosan is been stepping up their game as of late, but they are still at the level of HAAS or Mazak with regards to machine over capabilities. In conversations with 10 different companies over the last month I have heard of over 100 new machines being purchased in the next 6-12 months. I am aware of 2000 projects being onshored or reshored back in the USA. The manufacturing community as a whole is suffering from something so simple with regards to what you are fighting.  It is the lack of consistency using the same Fanuc control across many different builders. If Fanuc would demand and provide a testing process to certify builders are configuring their machines to use their controllers correctly then many of the problems facing Manufacturing as a whole would be reduced. Once it is figured out and a machine is running like it should anyone with a 5 Axis machine forgets all the work and effort it took for get them to that point. Take a machine with a correctly configured Camplete process. Those programmers in all reality have it easy. Take someone like yourself who is working their way through these issues you are gaining way more insight into the steps needed to get it correct. Problem is people like James, Colin, and others who know this stuff as well as they do are not a dime a dozen they are becoming one in a thousand to maybe as much as one in every ten thousand. With under 3 million people in manufacturing in the United States.