Right angle head on Haas VF-3?

[Darin]

Hello,

 

We have a part that is going to need a right angled head on our Haas.. I know how to program it in Mastercam using a Router post and it just routates the plane with aG17.... but how does it know the length of the tool or where to set it? The X0,Y0, is center of the part (See picture) and the Z0 is top of part... Do I just touch the tool from the top of the part and move down half the dia of the tool? But how does it know the length from the center of the right angled head to the tip of the tool? Make sense?

 

 

 

 

 

Thanks

[mkd]

router post is prolly a great starting point, although i use MPMaster functionality.

let's see if i remember correctly, as its been a few years:

put edge finder or indicator in right angle head and find z0

set this as TLO

in mastercam set you tool length to distance from SPINDLE centerline to tool tip. the post will use this to offset your x or y.

 

 

there are several other ways of accomplishing this. one way is to G92 off a tooling ball. i've used this recently for a prototype part that needed 5 axis holes. i used a gerardi compound angle head and a head/head 5axis post. editing out the angle moves.

 

any ways, the pickup method needs to match the post (captain obvious, i know)

[Darin]

router post is prolly a great starting point, although i use MPMaster functionality.

let's see if i remember correctly, as its been a few years:

put edge finder or indicator in right angle head and find z0

set this as TLO

in mastercam set you tool length to distance from centerline to tool tip. the post will use this to offset your x and y.

 

 

there are several other ways of accomplishing this. one way is to G92 off a tooling ball. any ways, the pickup method needs to match the post (captain obvious, i know)

 

Great ... So is the tool length controlled here? (See picture) In the Machine Component Manager- Aggregate? So I need to know the center line of the head and from there to tip of tool? Pu it in the Tool Axis Length box? Does the machine view angle have to be 90 or 180? I have seen both.. There is a pic of the 90 deg head also..

[Darin]

Ok no matter what I put in the Tool Axis Length box I get no change in the G code... The .025 hole is located at X.150 Y-1.0 Z2.8178 normal for top veiw in Mastercam.. Below is the code it creates.. Why isn't the Z changing when I chnge the Tool Axis Length box dimension? What am I doing wrong? For some reason it posts out X is now Y and Y is now Z but it has also another Z that would be normal if there is no right head... Isn't also supposed to be G19 instead of G17?

 

 

 

O0042 (15-422803-00 RB RIGHT ANGLE HEAD)

(RIGHT ANGLE HEAD)

(RIGHT ANGLE HEAD OPPERATION LAST OPP)

(INITIAL BUILD)

(PROGRAM - 15-422803-00 RB RIGHT ANGLE HEAD.NC)

(DATE - JAN-30-2013)

(TIME - 3:57 PM)

(T3 - 180.00 / 90.00 - STATION # - H3 - D3 - D0.0200")

N100 G00 G17 G20 G40 G80 G90

N110 G91 G28 Z0.

N120 T3 M06 (180.00 / 90.00 - STATION #)

N130 (MAX - Z.175)

N140 (MIN - Z-.025)

N150 G00 G17 G90 G54 X-1. Y2.8178 S3000 M03

N160 G43 H3 Z.175

N170 G94 G01 Z-.025 F5.

N180 G00 Z.175

N190 M05

N200 G91 G28 Z0.

N210 G28 Y0.

N220 G90

N230 M30

[mkd]

try in your tool definition itself, i'm thinking the "overall" length.

it depends what the post is setup for.

some posts you can enter it right in your "misc values"

[Darin]

try in your tool definition itself, i'm thinking the "overall" length.

it depends what the post is setup for.

some posts you can enter it right in your "misc values"

 

Tried both nothing changes the output of the code...

[TheePres]

The router post that I modified has a switch to enable or disable tool length. I will look for switch name 1st thing in morning.

[mkd]

thanks theepres.

 

 

use_oal : no$ #Scale coordinates to tool length with Aggregates

 

maybe this is the ticket for generic fanuc 4xrouter.pst

[mkd]

change no to yes

[Darin]

The router post that I modified has a switch to enable or disable tool length. I will look for switch name 1st thing in morning.

 

I started with a MRrouter X6 post in Mastercam.. I have tried changing the area in the post where it says set height height offset with tool in vertical postion and #Override Work Offset with Aggregate Offset Register Tried both of those and it doesn't chnge the code..

 

 

 

 

ug4$ : 1 #Debug output with the tilde '~'.

#A value greater the zero applies the variable formatting with

#debug output (default is typically FS 1 but not a guarantee).

#A value of zero gets the value directly with NO formatting.

linktolvar$ : 0 #Associate X tolerance variables to V9- variable?

linkplnvar$ : 0 #Associate X plane specific variables to V9- variable?

skp_lead_flgs$ : 0 #Do NOT use v9 style contour flags

bdrl_use_lead$ : no$ #Output the lead drill as drill position w/block drill

use_ra_offs : yes$ #Override Work Offset with Aggregate Offset Register

use_oal : yes$ #Scale coordinates to tool length with Aggregates <--------------------------- Put this to yes no change in code ---------------------------------->

use_g8 : yes$ #Use G8 P1 for Fast corner (adv preview) function?

use_dc : no$ #Output codes to raise and lower dust cover?

use_tl_select : yes$ #Use tool code string select for drill block?

use_hd_select : yes$ #Use tool code string select for multi-heads?

set_g43_vert : 0 #Aggregate - set height offset register with tool in vertical position? <--------------------- Changed this line to 0,1,2 no change--------------------->

# 0 = No, set in horizontal position

# 1 = Yes, set in vertical position

# 2 = Set in horizontal if right angle aggregate, vertical if tilting aggregate

dual_table : no$ #Set to yes to enable misc integer option

use_brush_ht : no$

get_1004$ : 1 #Find gcode 1004 with getnextop?

rpd_typ_v7$ : 0 #Use Version 7 style contour flags/processing?

strtool_v7$ : 2 #Use Version 7+ toolname?

tlchng_aft$ : 2 #Delay call to toolchange until move line

cant_tlchng$ : 1 #Ignore cantext entry on move with tlchng_aft

newglobal$ : 1 #Error checking for global variables

getnextop$ : 1 #Build the next variable table

tooltable$ : 3 #Pre-read, call the pwrtt postblock

rotaxtyp$ : 999 #Rotary Axis Override

cutpos2$ : m_one #Disable cutpos2 if not 4 axis, saves time

[Darin]

It says this in the MRrouter post but I don't get any change in the code when I set these up... Shouldn't I see a change in the code somewhere for it compensating for the center of the head to the tip of the tool somehwere in the code?

 

 

# - Modified position shifting for aggregates -

# If use_oal is set to yes$, XYZ values are shifted based upon tools overall length value and aggregates "Tool Axis Length"

# value (if defined). The aggregates "Tool Axis Length" value is the fixed "gauge length" from pivot point to collet face.

# Setting this value in the aggregate definition allows the end user to set the tools overall length value from collet face

# to tool tip rather than calculating from pivot point to tool tip every time the tool is changed.

# set_g43_vert controls how the aggregate tool is touched off on the machine (ignored when use_oal = no):

# 0 = Set in horizontal position (Centerline of tool)

# 1 = Set in vertical position (Tool tip)

# 2 = Set in horizontal position if fixed right angle aggregate, vertical position if compound angle aggregate -

# post determines based upon aggregate type set in aggregate component.

[Darin]

Ok I think i figured it out.. It was my plane it was set wrong... I set it to top WCS and right side both Tool Plane and Construction plane and now I get the correct code when I change the tool axis length box. But it is posting a G19 instead of a G17... Is this right?

 

 

 

 

N100 G19 G20 G90 G40 G80 G64 G49 G0 M05

N110 G8 P1

N120 G90 M05 Z0

N130 G52 X0. Y0. Z0.

N140 T5 M6

( RIGHT ANGLE HEAD )

( RIGHT ANGLE HEAD OPPERATION LAST OPP )

( INITIAL BUILD )

( 1ST SET - HELIX BORES THE .030 & .035, DIA HOLES WITH 90 DEG HEAD )

N150 G0 G90 X7.175 Y-1. C0.

N160 S3000 M3

N170 G43 H5 Z2.8178

N180 G1 X7.15 F40.

N190 G41 D5 Z2.8028 F15.

N200 Z2.7878

N210 G3 X7.149 Z2.8478 J0. K.03

N220 X7.148 Z2.7878 J0. K-.03

N230 X7.147 Z2.8478 J0. K.03

N240 X7.146 Z2.7878 J0. K-.03

N250 X7.145 Z2.8478 J0. K.03

N260 X7.144 Z2.7878 J0. K-.03

N270 X7.143 Z2.8478 J0. K.03

N280 X7.142 Z2.7878 J0. K-.03

N290 X7.141 Z2.8478 J0. K.03

[EX-wccprogrammer]

I think that you guys are over complicating this. I just put each angle head tool on its own work offset, and have the setup guy set the work offset at the tip of the tool.

[CJep]

I think that you guys are over complicating this. I just put each angle head tool on its own work offset, and have the setup guy set the work offset at the tip of the tool.

 

Second that,... I would add that I set the Z in the in the offset registry for that tool as the center of the tool