Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

bridgemill 90 deg head tool length compensation


FTI2007
 Share

Recommended Posts

I have a Ameraseiki bridgemill with a 90  deg head and fanuc control.  When I machine the 90 degrees faces its fine. But when I go to mill a 45 deg face meaning that  I'm cutting in X and Y at the same time I'm having trouble. First my post was not outputting the G44/G43 and the H command when doing the 45 degree faces.  So I got my post updated but now the machine is alarming out when It sees more than 1 axis with the tool length compensation.  If I run it without the tool length comp  and adjust the depth for my tool length  it cuts fine.  and if  I edit it so it only compensates 1 axis its not in the right position.     i hope this makes sense.   any ideas????

 

T1 M06(6" FACE MILL)
M200 C225.
M01
G17
G00 G59 G90 G44 H1 X-19.434 Y-13.4214       ( it gives alarm----- tool comp command more than 2 axis) 
Z2.475
M08
X-11.8327 Y-5.82
G01 X-11.5922 Y-5.5795 F30.
X-5.3444 Y-11.8274 F65.
X-5.5212 Y-12.0042 F50.
G00 X-13.1862 Y-19.6692
M09
G91 G00 G28 Z0.
M30

 

thanks 

 

 

90 deg face 45.JPG

Link to comment
Share on other sites

In the posts I've put together for this kind of stuff

the tool length offset is the distance to the centerline of the right angle head spindle

It would be the same for every tool.

The tool length is handled by an  gage length input during posting

The gcode is driving the C/L of the spindle, just like any other tool

Link to comment
Share on other sites

With the Fanuc control, you can only apply Tool Length Compensation (G43) on a single Linear Axis. What you can compensate for depends entirely on the options installed on your control.

Typically we still use G43 Zx.x Hxx for the vertical distance between the Tool Centerline, and the Gauge Point on the machine Spindle Face. (Machine Z Shift)

Most of the Fanuc controls I've run use G45/G46 (+ or - Axis Shift) or G47/G48 (double + or - Axis Shift), and either an X or Y value and the Dxx comp register value. (Machine X or Y Shift)

What the G45 does is "shift" the driven point of the control from the Spindle Centerline in X or Y, to the distance in the Dxx register. (Register is typically offset by '30' or '50', since you need a CRC register, and a Z Shift distance. So T05 would use D05 for CRC, and D55 for X or Y Shift.)

The Axis Shift is only able to be applied along a single Linear Axis of the machine. This allows you to accurately apply a shift to the Tool Tip, using Offset Registers on the machine, and will still let you use G18 or G19, with G41/G42 Cutter Compensation. The problem with this is that you are limited to doing Planar work, at one of 4 possible 90 Degree orientations. You won't be able to compensate for a non-planar angle with this method.

This is really a limitation of the Fanuc Control, and the options you have available.

What you are looking for is Tool Center Point Control, which allows what is essentially "5 Axis Tool Length Compensation". (G43.4 or G43.5) This is however, an option that not many people order when buying a machine like this. This option is typically used with 5 Axis Vector based paths though. (Point to Point)

The option you really want to use is G68.2 Coordinate Rotation, to rotate and/or translate the Work Offset location and orientation. This aligns the rotated coordinate system to have the "Z Axis" aligned to the Tool Vector, and the Y Axis "lowered" by the amount of the "Machine Z Shift", to account for the distance between spindle gauge face and the angled tool centerline. By rotating the CSYS, the axis system in the Control's memory is aligned so the CSYS Z Axis is aligned with the rotated tool axis. This let's you use "G17", with G02/G03 Arcs, G40/G41/G42 Cutter Compensation, and G43 Zxx Hxx for Tool Length. 

Link to comment
Share on other sites
15 hours ago, gcode said:

In the posts I've put together for this kind of stuff

the tool length offset is the distance to the centerline of the right angle head spindle

It would be the same for every tool.

The tool length is handled by an  gage length input during posting

The gcode is driving the C/L of the spindle, just like any other tool

With our machine we touch off tools like normal without the 90 DEG head on. then when we put the head on those offset lengths are transfered to the head. the post compensates for the additional length the head adds.   I only have problems when  face milling in 2 directions where it needs to apply the offset to 2 axis at the same time.  

thanks

Link to comment
Share on other sites
12 hours ago, Colin Gilchrist said:

With the Fanuc control, you can only apply Tool Length Compensation (G43) on a single Linear Axis. What you can compensate for depends entirely on the options installed on your control.

Typically we still use G43 Zx.x Hxx for the vertical distance between the Tool Centerline, and the Gauge Point on the machine Spindle Face. (Machine Z Shift)

Most of the Fanuc controls I've run use G45/G46 (+ or - Axis Shift) or G47/G48 (double + or - Axis Shift), and either an X or Y value and the Dxx comp register value. (Machine X or Y Shift)

What the G45 does is "shift" the driven point of the control from the Spindle Centerline in X or Y, to the distance in the Dxx register. (Register is typically offset by '30' or '50', since you need a CRC register, and a Z Shift distance. So T05 would use D05 for CRC, and D55 for X or Y Shift.)

The Axis Shift is only able to be applied along a single Linear Axis of the machine. This allows you to accurately apply a shift to the Tool Tip, using Offset Registers on the machine, and will still let you use G18 or G19, with G41/G42 Cutter Compensation. The problem with this is that you are limited to doing Planar work, at one of 4 possible 90 Degree orientations. You won't be able to compensate for a non-planar angle with this method.

This is really a limitation of the Fanuc Control, and the options you have available.

What you are looking for is Tool Center Point Control, which allows what is essentially "5 Axis Tool Length Compensation". (G43.4 or G43.5) This is however, an option that not many people order when buying a machine like this. This option is typically used with 5 Axis Vector based paths though. (Point to Point)

The option you really want to use is G68.2 Coordinate Rotation, to rotate and/or translate the Work Offset location and orientation. This aligns the rotated coordinate system to have the "Z Axis" aligned to the Tool Vector, and the Y Axis "lowered" by the amount of the "Machine Z Shift", to account for the distance between spindle gauge face and the angled tool centerline. By rotating the CSYS, the axis system in the Control's memory is aligned so the CSYS Z Axis is aligned with the rotated tool axis. This let's you use "G17", with G02/G03 Arcs, G40/G41/G42 Cutter Compensation, and G43 Zxx Hxx for Tool Length. 

Ill have to look into this some more and see if we have any of the options you mentioned.  I would guess that we do not. 

 

thanks

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...