Right angle head setup

[JB7280]

I have a right angle head in an HMC.  I've only ever used it via hand-coding.  How difficult is it to get working properly in Mastercam?    I followed a video I found on youtube, but I didn't have a lot of luck.

 

Reseller says I would have to use a router post, is that correct?

[crazy^millman]

A few questions need to be answered first. What post are you using? What direction is the Tool Pointed in on the HMC X+, X-, Y+ or Y-? Have you tried defining an aggregate head in the MMD?

A router Post will help get the work done on the cheap for upfront cost, but a good 3rd Party post will do it and done. With a router post you will have to spend some time dialing and proving everything out. With a 3rd Party post once you answer the basic setup questions do a few test cuts should be dialed in and good to go. The real thing is what are you trying to do with the RAH? Simple drilling and other things? Are you looking to set someone hair on fire and machine some really crazy features? Keeping the RAH in one orintation or will be spinning it around to different axis?

Simple RAH work can be programmed in a normal HMC. You just have to trick Mastercam with toolpaths to get the code. Once you work out the Center line of the RAH to the Gauge Length then basic programming can be done. It is when you try to get into more complex work it where it gets tricky and want a good post to make it such.

[JB7280]

1 minute ago, crazy^millman said:

A few questions need to be answered first. What post are you using? What direction is the Tool Pointed in on the HMC X+, X-, Y+ or Y-? Have you tried defining an aggregate head in the MMD?

A router Post will help get the work done on the cheap for upfront cost, but a good 3rd Party post will do it and done. With a router post you will have to spend some time dialing and proving everything out. With a 3rd Party post once you answer the basic setup questions do a few test cuts should be dialed in and good to go. The real thing is what are you trying to do with the RAH? Simple drilling and other things? Are you looking to set someone hair on fire and machine some really crazy features? Keeping the RAH in one orintation or will be spinning it around to different axis?

Simple RAH work can be programmed in a normal HMC. You just have to trick Mastercam with toolpaths to get the code. Once you work out the Center line of the RAH to the Gauge Length then basic programming can be done. It is when you try to get into more complex work it where it gets tricky and want a good post to make it such.

I am using a slightly modified version of the MPMaster post.  Just drilling some holes.  Nothing too crazy.  The right angle head is only being used with the drill pointing in the Y+ direction.  I did try building an aggregate head, but I'm not sure if I did it correctly, because I get the achievable toolplane error when I try to post.  Nobody's hair needs to be set on fire at the moment, but I just thought it would be a good option to have in the future, since we have the head already. 

[crazy^millman]

1 hour ago, JB7280 said:

I am using a slightly modified version of the MPMaster post.  Just drilling some holes.  Nothing too crazy.  The right angle head is only being used with the drill pointing in the Y+ direction.  I did try building an aggregate head, but I'm not sure if I did it correctly, because I get the achievable toolplane error when I try to post.  Nobody's hair needs to be set on fire at the moment, but I just thought it would be a good option to have in the future, since we have the head already. 

The trick then is to make a Toolpath where you are tricking the post to give you the output you want. If you are okay with long code then a simple Point or 3D contour toolpath will output the code needed to drive the RAH. Too much going on now to put together a sample file, but if you put together a sample file then I am sure someone would be glad to expand on what I am saying. If someone else doesn't then as time permits I will be glad to put toolpath to the file to show you what I mean. Make it a Z2G so I can test the outputted code to make sure we are getting what I am thinking.

To anyone following this topic. Machinesim setup by a 3rd Party can simulate RAH in these situations when the POST it tied Machinesim.

[JB7280]

19 minutes ago, crazy^millman said:

The trick then is to make a Toolpath where you are tricking the post to give you the output you want. If you are okay with long code then a simple Point or 3D contour toolpath will output the code needed to drive the RAH. Too much going on now to put together a sample file, but if you put together a sample file then I am sure someone would be glad to expand on what I am saying. If someone else doesn't then as time permits I will be glad to put toolpath to the file to show you what I mean. Make it a Z2G so I can test the outputted code to make sure we are getting what I am thinking.

To anyone following this topic. Machinesim setup by a 3rd Party can simulate RAH in these situations when the POST it tied Machinesim.

That's sort of what I did.  I used a point toolpath.  but then I posted and put it into a manual entry, then used a variable so that the operator has somewhere to enter the new tool length when they need to change the drill.  Then used that variable for the positioning in the g-code...like so....

G01 Y[-1.7015-#700]F1.2
G00 Y[-1.8315-#700]
G01 Y[-1.6715-#700]
G00 Y[-1.8315-#700]
G01 Y[-1.6415-#700]
G00 Y[-1.8315-#700]
G01 Y[-1.6115-#700]
G00 Y[-1.8315-#700]
G01 Y[-1.5815-#700]
G00 Y[-1.8315-#700],

 

Wouldn't work as well for a more complex toolpath, but for this, it works.

[Greg Williams]

Mastercam Support the RAH. I did this for an Okuma

G00 G17 G94 G40 G80 G90
G21
N4 G00 Z999.
(OPERATION NUMBER - 2)
(WCS NAME - TOP)
(TOOLPLANE NAME - HOLE-2)
G116 T4 ( 0.00 / 90.00 - STATION NO -)
(VC1 = THE X OFFSET)
(VC2 = THE Y OFFSET)
S2652 M03
G15 H1
(MAX | Z150.)
(MIN | Z-118.001)
G00 G90 X=VC1+416.433 Y=VC2-201.491
G56 H4 Z150. M08
G01 Z-12. F5000.
X=VC1+418.965 Y=VC2-189.046
X=VC1+419.364 Y=VC2-187.087 F265.2
X=VC1+418.965 Y=VC2-189.046 F5000.
X=VC1+419.364 Y=VC2-187.087
X=VC1+419.762 Y=VC2-185.127 F265.2
X=VC1+418.965 Y=VC2-189.046 F5000.
X=VC1+419.762 Y=VC2-185.127
X=VC1+420.161 Y=VC2-183.167 F265.2
X=VC1+418.965 Y=VC2-189.046 F5000.

**********************************

X=VC1+424.946 Y=VC2-159.649
X=VC1+425.345 Y=VC2-157.689 F265.2
X=VC1+418.965 Y=VC2-189.046 F5000.
X=VC1+425.345 Y=VC2-157.689
X=VC1+425.743 Y=VC2-155.729 F265.2
X=VC1+418.965 Y=VC2-189.046 F5000.
X=VC1+425.743 Y=VC2-155.729
X=VC1+426.142 Y=VC2-153.769 F265.2
X=VC1+418.965 Y=VC2-189.046 F5000.
X=VC1+426.142 Y=VC2-153.769
X=VC1+426.341 Y=VC2-152.789 F265.2
X=VC1+418.965 Y=VC2-189.046 F5000.
X=VC1+416.433 Y=VC2-201.491
Z150. M09
M05
G00 Z999.
S300 M03
M12 (TOOL CLEANING AIR BLOW)
G04 P3.0
M09
M05
G00 Y999.
G90
M02
%