G43.4 where should it be?

[Jean-Simon]

Good morning all, I'd like to know where my G43.4 should be: If I put it after my XY positionning, my entry point isn't compensed so it enters far out and if I output it before "illegal command in G43.4" which I assume you can't have rapids in RTCP. I'm doing a cone test cut (Swarf 5x) on a 5x SNK milling with Fanuc 31i-A5 control. I'm also using G05.1. Any onput would greatly be appreciated.

 

Have a good day!

 

Simon

[MLS]

Here is an example of where we output it for a Makino Mag3. We have a motion analysis segment where it positions X and Y; then Z(with G43.4 & H Comp); then Recalls the X, Y, Z, and positions the C, A move.

 

Note: we do not use Mastercam posts.

 

S20000M03M08

G90G54

G00X-107.1998Y-12.7554

G05P10000 (Super GI Makino)

G43.4Z5.H01

G00X-107.1998Y-12.7554Z5.A.0C.0

Z3.5

 

This particular toolpath is a 0,0,1 tool axis, but regardless the format is the same for us.

[Jean-Simon]

Thanks it makes sense!

 

JS

[MMT-USA]

MLS,

 

It looks like you are using TCPC Type 1. Have you tried type 2?

[Jean-Simon]

Thanks a lot I'm back from the machine and and do exactly what I want. We have other 5x machines that needs to be program from pivot points and inverse time so these options are new to me. It looks much simpler to have a smooth toolpath that way.

MMT-USA I didn't try the type 2 (g43.5) roughly what is better?

 

Such a great place to hang around!

 

Thanks again!

 

JS

[MLS]

MMT,

I wasn't here when they set up the protocol for that machine, so I don't know if they tried that or not. What are the differences?

 

JS,

Glad that worked. Cheers

[MMT-USA]

Basically TCPC is an option from Fanuc that instead of feeding the control direct XYZ ABC machine coordinates, you instead feed it cutter location coordinates that are always relative to the part. The controller will make the necessary calculations on the fly to account for the effects of the part rotation.

 

Some maybe familiar with this on the Siemens control called Traori or RTCP.

 

Programs using this function in Type 2 are independent of machine kinematics and machine zero. This means if you change the location of the part on the machine you do not need to repost it. You can also use the same program on a machine with completely different kinematics since the controller will make the necessary calulations to adjust for this.

 

TCPC automatically adjusts the axis feeds to make sure that the feedrate of the tool is relative to the part. No need for Inverse Time Feed G93

 

The controller modifies the axis motion so the tool follows a straight line relative to the part avoiding linearization errors do to kinematics.

 

One problem is this function is not completely developed for the Fanuc and has some programming restrictions.

 

The Siemens is proven with really no limitations.

 

Hopefully we'll see more Fanuc users using type 2 in the near future. I believe Fanuc has added to this developement but unfortunately not too many customers in the world use it do to its current development stage.

 

sorry havent had my coffee yet !

[MLS]

I see.

 

Makes sense. I doubt they ever tried to use it. At this point the workload for those machines prevents us from doing any testing, but I'll keep that in mind should the machine ever have a free day. I'm thinking this would be MORE of an advantage on a table/table type machine as opposed to a head/head(nutator) type machine.

 

We are in the process of testing our first machine with a Siemens control. So if I understand the Traori function correctly it more or less does all the mathematics to calculate the tip of the tool and compensate it's motion at all times related to all axes. As opposed to relying on the code to supply part of that information. It would make the programmer's life easier. heh

 

Thanks for the info

[MMT-USA]

You got it! Good luck

[Jean-Simon]

Thanks for explanations, sorry for the delay, I was out of the office (in a Siemens aerospace workshop) they were presenting their 840D.

 

Thanks again!

 

Simon