5-axis turning

paehv · 2015-12-21 18:58:19

For a new Grob machine I am creating the vericut controller (sinumerik 840d sl) and machine. This is a 5-axis millturn machine.
When doing oriented turning we use CYCLE800 for positioning the A-axis. The B-axis is the turning spindle.
I got this running in vericut without any problems.
For simultanious turning (drive X, Z and A-axis simultane by using traori(2)) I get -for soms tools- the error "...off turning plane..."
The insert lies in the xz plane and the y position is 0
For some tools this only happens with spindle orientation 270 degrees and not on 90 degrees.
All tools work without any trouble when using cycle800.
Does anyone have an idea what might be causing this?

Verifun · 2015-12-21 19:12:04

Patrick,

We use the following macros to mimic simultaneous axes during turning:

CGTECH_MACRO "DYNAMICTOOLTIPONOFF" "" 1
CGTECH_MACRO "DYNAMICTOOLTIPADJUST" ""
CGTECH_MACRO "RTCPCONTOUR" "" 1

And these to disable it:

CGTECH_MACRO "DYNAMICTOOLTIPONOFF" "" 0
CGTECH_MACRO "RTCPCONTOUR" "" 0

Never had any "...off turning plane..." except when there was indeed a problem in our tool assembly or Y was not at 0.

But we use it mostly with WFLs, with the typical B head / C table (Chuck) configuration, similar to Mazak Integrex...

paehv · 2015-12-22 07:52:16

Hi Daniel,

I've been playing with these macros. The where actually activated when TRAORI(2) is turned on.
It turns out that when I set the macro DYNAMICTOOLTIPONOFF to 0 instead of 1, every tool is OK.
When it's set to 1, some tools get a small offset in the Y-direction.
Looking thru the docs, it may be because I don't have the tool origin in the center of the insert radius.

I'm wondering why this setting would be needed anyway, if the tool orientation is fixed and the part (table) can swivel. In NX CAM the toolpath calculated already takes this orientation into account.

This is our first turning machine that has 5-axis turning capabilities (https://youtu.be/8UEzDhmiFq0), so I'm still trying to figure out what would be the best approach on tool offsets and driven points.
On your WFL do you use driven point #9 (center of insert radius)?
Do you use radius compensation, or do you adjust X,Z tool offsets.
How do you manage tools with multiple driven point, like grooving tools?

Any tips will be appreciated.

Verifun · 2015-12-22 23:53:30

Before 7.3.2 VERICUT did not support the driven point off the center for B axis turning, on indexed or contouring mode. CGTech made it happen for us... It works now with CUTCOM and multiple driven points...

I´ve seen this small displacement along Y when G18 is not the current plane... Are you sure you´re calling it before calling the macros?

The way we do it is in our tool change sub we check the tool type we are loading and then load the current plane selection command... G17, G18...

After that we call the macros...

These 3 ones must be called after each B axis repositioning... We do it within our tool change sub... then your driven point will be updated... even if it´s not set to be in the center of the tool radius...

CGTECH_MACRO "DYNAMICTOOLTIPONOFF" "" 1
CGTECH_MACRO "DYNAMICTOOLTIPADJUST" ""
CGTECH_MACRO "RTCPCONTOUR" "" 1

VERICUT can support each and every feature you´re looking for...

Let me know how else I can be of help....

Last edited by Verifun (2015-12-23 00:02:08)

Verifun · 2015-12-23 00:07:37

paehv wrote:

Hi Daniel,
I'm wondering why this setting would be needed anyway, if the tool orientation is fixed and the part (table) can swivel. In NX CAM the toolpath calculated already takes this orientation into account.

You have a good point here. If the tool only moves along Z, like in a regular lathe (X becomes Z in that Grob), then you need RPCP macros instead of RTCP.

Try CGTECH_MACRO "RPCPCONTOUR" "" 1 instead of CGTECH_MACRO "RTCPCONTOUR" "" 1

Last edited by Verifun (2015-12-23 00:09:36)

Verifun · 2015-12-24 16:05:23

VERICUT as you know do support a combination of RTCP and RPCP. I think even tough your tool only moves along a linear axis, you may need RTCP to handle it.

JM2C...

VERICUT Users' Forum

#1 2015-12-21 18:58:19

5-axis turning

#2 2015-12-21 19:12:04

Re: 5-axis turning

#3 2015-12-22 07:52:16

Re: 5-axis turning

#4 2015-12-22 23:53:30

Re: 5-axis turning

#5 2015-12-23 00:07:37

Re: 5-axis turning

#6 2015-12-24 16:05:23

Re: 5-axis turning

Board footer