Multus Tool setting

[steve.edmshop]

I wonder if someone can help.

A client of mine has a B300 with a Renishaw automatic toolsetter. If he sets a turning tool, no other edge positions are stored. In other words there is no offset stored when the head is a different angle. Consequently he has to set the tool at each angle he wishes to use that tool at.

Surely there is a function where the machine can calculate the new edge position for different head angles if you only set the tool in one position?

I would really appreciate a step by step procedure on how to do this.

Thanks in advance.

steve@edmshop.co.za

[DIFF OVER]

contact your Okuma dist and get the Multi Func Asst 2.6 manual.

when you touch off but not with the touch setter, you must select the Auto Cal button.

TOOL OFFSET AUTO CALCULATION PATTERN parameter.

Tool offset automatic calculation selection
Tool offset automatic calculation selection ? 0: Automatically calculate all positions (Default setting)
Setting range: 0 to 255 ? Other than 0: The automatic calculation will be executed by combining numbers.
Automatic calculation will not be performed if only one set is selected.

0: Perform the automatic calculation for all forms (Default setting)
1: Main spindle reference position A
2: Main spindle orthogonal position A
4: Sub spindle reference position A
8: Sub spindle orthogonal position A
16: Main spindle reference position B
32: Main spindle orthogonal position B
64: Sub spindle reference position B
128: Sub spindle orthogonal position B

Example:
If the value obtained by adding the 1st spindle reference position A “1” and the 1st spindle orthogonal position A “2” (1 + 2 = 3) is set at the parameter, the orthogonal position A will be automatically calculated when the reference A is offset, and vice versa.

[steve.edmshop]

Hi,

Thanks for your reply.

I have now set a 45 degree tool at BT=0. The length of the tool is 210mm (Z) and the X axis value is 0.0. I set the edge postion P=5 and the X rad to 0.8 and the Z rad to 0.8.

I then auto-calculate. When I move to BA=45 G52, and go to the face of the job (Z0) the tool stands 0.96mm in front (i.e Z0.96) and if I move to X50.8 the machine cuts a diameter of 49.5.

It's as though the angle the machine is moving to is wrong (something like 47 degrees)

Has anyone else had this problem?

Thanks for your help.

Regards

Steve (steve@edmshop.co.za)

[DIFF OVER]

BT=0 and BT=1 are to used only at Base and VERTICAL position.

G52 for live tools only.

a 45 degree tool will act differanty at M602 or M603.

from the Multi Func Assistant:

Note: for 45° lathe tools: When using lathe tools at an angle (typically 45°) the touchsetter or Auto Calc will give some unexpected results.

[steve.edmshop]

Firstly, thanks again for your support.

The problem I have is that even live tooling is moving to the wrong position when I rotate the spindle. If I set a drill in the BT=0 Position and rotate to BA=45 G52 and want to drill, I need to set the X and Z position for the drill at 45 degrees and as you can imagine this is hit and miss.

I'm no Okuma expert, but surely this isn't right? Could the "knuckle" position be incorrect in the parameters? If they are how do I rest them?

Thanks again.

[DIFF OVER]

You are SLOPE MACHINING?

B-Axis (Slant Machining) Operation
M-Codes:
G174
Zero point shifting
G175
Zero point shifting cancel
G126
Slant machining mode off
G127
Slant machining mode on (B***.***)

Address Characters:
SX VZSHX (Shift X)
SZ VZSHZ (Shift Z)
SY VZSHY (Shift Y)



Notes:
• Slant machining mode is cancelled by <Reset>.
Program Example:

(30° angle drill; Shift 1.74" in X and 3.791" in Z)
MT=0101 (Tool #1)
M321
G0 X50 Z.5 TL=0909 BT=0 BA=30 G52 (Rotate B-Axis 30)
X5.0 Z.5
M110 (C-Axis Mode On)
G138 (Y-Axis Mode On)
G174 SX=1.75 SZ=3.791 (Zero Shift X and Z)
G127 B30 (Rotate Coordinates 30)
SB=500 M13
G0 X0.0 Y0.0 Z.1
G183 C0.0 X0.0 Y0.0 Z-.8 K0.0 D.25 L.5 F.01
G180
G0 Z1.
G126 (Cancel Slant Mode)
G175 (Cancel Zero Shift)
G136 (Cancel Y-Axis Mode)
M12
M109 (Cancel C-Axis Mode)
X50 Z1.0
TC=1 (Index Turret to Base Position)
M1

[mally38]

when I use a 80deg tool that is a 45 deg holder I will touch it off going BA=45 deg then touch both edges X and Z when you use it this way your offset adjustments are in Base
I really like these tools very ridged.
Tim