Project of the Month built by Johno1958

Help Support Home Model Engine Machinist by donating using the link above or becoming a Supporting Member.
Home Model Engine Machinist > CNC and 3-D Printers > Software and Programming > Mastercam Mill 9.1

Thread Tools
Old 08-14-2012, 06:26 PM   #11
Join Date: Aug 2012
Posts: 5
Liked 1 Times on 1 Posts


Originally Posted by atheras29 View Post
Post from Master Cam the existing post again and before sent it to mill change the diameter of the existing # tool under description of tool

( make it smaller off .0039'')

second line under the first G codes

if you have any problems please post a picture of the post to help you

good luck
This is a bandaid fix. not proper method. You should add an entry motion. Your controller is throwing an alarm because you cannot start a cutter comp on an arc motion. it must lead in straight to activate the cutter comp and arc after its active.

Also use wear comp, and do not use any geometry (radius) in the control when setting up. Ie you should set the tool length only, no radius. Then use your wear comp value to adjust the .0039".

It's been a long time since I used/trained mc9 so I cant tell you where the exact commands are, but you should have lead in lead out options, use start at centre and perpendicular entry. I have MCX6 currently.

Justin_Sane is offline  
Reply With Quote
Old 08-14-2012, 09:14 PM   #12
kvom's Avatar
Join Date: Jun 2008
Posts: 3,079
Liked 612 Times on 484 Posts
Likes Given: 286


WRT not using the radius in the control: I believe this means you tell MC to offset the toolpath rather than the control, so define the tool in MC.
kvom is offline  
Reply With Quote
Old 08-14-2012, 09:59 PM   #13
Join Date: Aug 2012
Posts: 5
Liked 1 Times on 1 Posts


The way mastercam outputs the toolpaths with the comp options is basically this,

-computer (no comp command, coordinates are tool centreline)
-wear (comp command g41/42, coordinates are also tool centreline, but tool shifts to the proper side by the amount of wear comp in control, usually a very small number), leave the geometry (rad/diameter) column to zero on the control of the machine)
- control (comp command g41/42, outputs coordinates of the geometry, this is used when you are entering the tool radius or diameter (depending on control settings of machine) into the tool geometry, this allows you to change the tool from say 3/4" to 1/2" at the control rather than by changing the toolpath. this can cause issues though if you allow the operator to decide what tool diameter to use. This can also use the wear comp on the machine to make minor adjustments with this method.

You can tell mastercam that the tool is a smaller size to adjust the toolpath with comp set to computer, however the next time you run it with a brand new tool, you might overcut your part.

use wear comp with a lead in motion on the helix and you can make minor adjustments while still retaining the proper programmed coordinates. That is pretty much the industry standard way. Most of my customers use it that way anyways

also one of the previous comments suggested that an option may not be available. That would not matter as you can easily output point to point code that will do the same thing. all the helical or tornado option is, is a macro canned cycle that does the cycle with a one line call. Very nice for when you want to punch a quick hand program on the control, but not necessary when using a CAM system.
Justin_Sane is offline  
Reply With Quote

Thread Tools

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
Mill-rite mill rebush Tools 4 05-11-2012 11:58 PM
Mastercam kustomkb Software and Programming 14 01-14-2010 01:25 PM
Tramming a small mill (Sherline mill) ttrikalin Tips and Tricks 9 11-22-2009 06:58 PM
Mastercam X2 help. Speedy Software and Programming 1 05-13-2009 11:44 AM
wanted mastercam book Speedy Buy / Sell / Trade / eBay 2 06-14-2008 10:13 PM

Newest Threads

- Top - Member List