tool diameter or radius?

This forum is for requests and queries about machine tool support for Vectric Products

tool diameter or radius?

Postby 4DThinker » Thu Jun 22, 2017 7:04 am

Wondering if the tool diameter or radius of the tool used in a toolpath being processed is passed to (available to) the post processor? If so, what is the variable name?

My goal is to do some probing in the X and Y directions with a touch plate to set my X and Y origin points for some jobs. Thinking I'll need to set tool radius compensation, so where/how do I acquire the current bit radius?

Thanks!
4D
4DThinker
Vectric Wizard
 
Posts: 981
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: tool diameter or radius?

Postby Adrian » Thu Jun 22, 2017 8:02 am

There is no documented variable for the tool radius/diameter but you could set it in the notes for the tool in the database and the post processor can pick it up from there.
User avatar
Adrian
Vectric Archimage
 
Posts: 7409
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: tool diameter or radius?

Postby 4DThinker » Thu Jun 22, 2017 8:16 am

Adrian wrote:There is no documented variable for the tool radius/diameter but you could set it in the notes for the tool in the database and the post processor can pick it up from there.
Thanks for your response, Adrian. We use end mills from a variety of manufactures and many vary slightly in diameter despite all claiming to be the same as what their packaging states. My tool database (in Aspire) has each tool generically described, and we caliper measure the actual bit when creating toolpaths. The real diameter gets edited just into the short entry for the current tool so as not to keep changing the main tool database. On our college servers the main tool database is frozen.

Where do I find it? How do I "pick it up"? Sorry for my ignorance here. I'm a post processor rookie.

4D
4DThinker
Vectric Wizard
 
Posts: 981
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: tool diameter or radius?

Postby Adrian » Thu Jun 22, 2017 8:49 am

The Post Processor editing guide is on the Aspire/VCarve/Cut2D Help menu if you haven't found it. The tool notes variable is [TOOL_NOTES].
User avatar
Adrian
Vectric Archimage
 
Posts: 7409
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: tool diameter or radius?

Postby ger21 » Thu Jun 22, 2017 12:47 pm

That's where G41/G42 comes in handy. :)
Gerry
ger21
Vectric Wizard
 
Posts: 854
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: tool diameter or radius?

Postby dah79 » Thu Jun 22, 2017 1:04 pm

4D,

Put this in your post processor file(s) header section and then what ever you have in your tool's data base 'notes section' will be inserted into your gcode file.

"( TOOL NOTES: [TOOL_NOTES] )"

Hope this is what you are after.
Attachments
PP modification.pdf
(23.62 KiB) Downloaded 34 times
Dave
dah79
Vectric Craftsman
 
Posts: 260
Joined: Thu May 14, 2015 12:23 am
Location: Bemidji, MN
Model of CNC Machine: FLA Saturn 4x4

Re: tool diameter or radius?

Postby 4DThinker » Thu Jun 22, 2017 2:29 pm

Thanks everyone for the tips.

I think I started out making my idea harder to accomplish than it needs to be.
I already set up my material in Aspire with an XY Datum offset of 1/2 my actual bit diameter. If the 3/16" bit is actually .1904 I use .1904/2 or .0952. When touching off X and Y I just want the edge of the bit to touch the -X and -Y edges of the material block. Using G38.2 with my touch plate it looks like I just need to add the touch plate thickness to wherever the bit is when probe contact is made to get it flush to the material in each respective direction.

I'm using LinuxCNC and will look into how it already probes for my Z datum using the touch plate.

4D
4DThinker
Vectric Wizard
 
Posts: 981
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: tool diameter or radius?

Postby TReischl » Wed Jun 28, 2017 6:57 pm

Measuring end mills with a "caliper" is not exactly very accurate. Even a micrometer is not all that good.

Some food for thought: It does not matter what the end mill measures across the flutes. What matters is how wide it cuts. When I really, REALLY need to cut accurately what I do is measure the width of a test piece carefully. Then I cut a slot (on a vector, not going round and round), then chop off the ends and put the two pieces together and measure them.

I also use this technique on the table saw to measure how wide the blade is cutting.

Oh, the point is that using a micrometer or caliper on a large surface is much more accurate than measuring across sharp flutes. Plus, if that end mill is not perfectly concentric measuring the flutes is not telling you much.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 1966
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset


Return to Post Processors

Who is online

Users browsing this forum: No registered users and 4 guests