Climb Mill On Vector

This forum is for general discussion regarding VCarve Pro
Post Reply
kstrauss
Vectric Craftsman
Posts: 188
Joined: Mon Apr 29, 2013 3:37 am
Model of CNC Machine: Tormach PCNC770
Location: Cobourg, ON, Canada

Climb Mill On Vector

Post by kstrauss »

The climb/conventional toggle seems to be ignored when machining ON an open vector (direction is honoured when left or right of an open vector and also works ON a closed vector).

I want to use a V-bit to chamfer the edges of features. I have created an offset path for the V-bit and cut ON it. This works fine other than the direction. If I use Allowance offset to move the point of the V-bit off the edge of the project then Vcarve uses the diameter of the V-bit to generate the path rather than just offsetting the point by the requested amount.

The only way that appears to work is to use Node Edit to reverse the direction of the vector. Is there an easier way?

tomgardiner
Vectric Wizard
Posts: 391
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Climb Mill On Vector

Post by tomgardiner »

When you think about it, if one side of a cut is climb cutting then the other side is conventional. That is why the option is nullified for cutting on the line. You do have the option however to change the direction of a cut on an open vector by changing the start point of the vector in node editing.

kstrauss
Vectric Craftsman
Posts: 188
Joined: Mon Apr 29, 2013 3:37 am
Model of CNC Machine: Tormach PCNC770
Location: Cobourg, ON, Canada

Re: Climb Mill On Vector

Post by kstrauss »

Of course but as I originally mentioned "I want to use a V-bit to chamfer the edges of features" so the tool is only cutting on one side. In my case climb versus conventional is meaningful.

tomgardiner
Vectric Wizard
Posts: 391
Joined: Thu Oct 02, 2014 1:49 pm
Model of CNC Machine: FMT Patriot 4 x8

Re: Climb Mill On Vector

Post by tomgardiner »

Sorry, guilty of skimming your post before responding. Nasty habit.
The only other way to do this I can think of is to profile outside and use an offset and start depth with a little math to achieve a chamfer. More work I think to achieve the club cut control. I'm not at my computer to test this.

User avatar
TReischl
Vectric Wizard
Posts: 3642
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Climb Mill On Vector

Post by TReischl »

kstrauss wrote:The climb/conventional toggle seems to be ignored when machining ON an open vector (direction is honoured when left or right of an open vector and also works ON a closed vector).
Does not appear to ignore it on my system???? I tell it to climb, it goes one direction, tell it to go conventional it goes the opposite direction. So it is not ignoring anything.

However, since it is on the line it has no way of determining which way is which so yes, you may need to switch the vector direction or just click the opposite to climb or conventional.

Think about it, YOU are telling the software it is ON the line, how is it supposed to know which way you want to go? Until you declare inside or outside it has no way of knowing. Computers are not that smart contrary to all the blather about "artificial intelligence" now available from a car dealer near you.
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
Leo
Vectric Wizard
Posts: 3071
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Climb Mill On Vector

Post by Leo »

You can set the diameter in tool data to .002 in the tool path dialog box. Then select outside milling. This will allow the climb mill to work for you.
Imagine the Possibilities of a Creative mind

www.leosworkshop.com

User avatar
TReischl
Vectric Wizard
Posts: 3642
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Climb Mill On Vector

Post by TReischl »

Leo wrote:You can set the diameter in tool data to .002 in the tool path dialog box. Then select outside milling. This will allow the climb mill to work for you.
I don't think that works for a v bit Leo. If you set it to a small value like you suggested then the maximum depth pass will be very small.

Example:
Capture.JPG
Then if you set it to a bit bigger, like .02 you get:
c2.JPG
Notice that the maximum pass depth is controlled by the diameter of the tool.
"If you see a good fight, get in it." Dr. Vernon Jones

ger21
Vectric Wizard
Posts: 1572
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Shelby Township, MI, USA
Contact:

Re: Climb Mill On Vector

Post by ger21 »

Just reverse the direction of the vector.
Gerry - http://www.thecncwoodworker.com

User avatar
Leo
Vectric Wizard
Posts: 3071
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Climb Mill On Vector

Post by Leo »

TReischl wrote:
Leo wrote:You can set the diameter in tool data to .002 in the tool path dialog box. Then select outside milling. This will allow the climb mill to work for you.
I don't think that works for a v bit Leo. If you set it to a small value like you suggested then the maximum depth pass will be very small.
Yes it will work.

Sooooo - set the stepover to .001 - this is a profile cut - not a pocket.

If he is setting a depth of cut on a profile toolpath it will offset the tool by .002 from tool centerline. The offset isn't really going to matter because is is so small of an amount. The depth will take care of itself and cut the chamfer - albeit, offset by .002

Now if this was V-Carving - it would not work.

EDIT IN:

OK so just reread your post. Maybe then, create a different tool. I have not tried any of this but there must be a way.

I will play with it at lunchtime

There are several way to skin this cat. All of which end up with the same result.
Imagine the Possibilities of a Creative mind

www.leosworkshop.com

User avatar
Leo
Vectric Wizard
Posts: 3071
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: Climb Mill On Vector

Post by Leo »

OK - it works by using a straight end mill, You just cannot see a chamfer on the part

I will retract my earlier recommendation about changing the tool diameter

Normally, I offset the toolpath by a couple of thou, but don't pay attention to cutter direction.
Imagine the Possibilities of a Creative mind

www.leosworkshop.com

User avatar
TReischl
Vectric Wizard
Posts: 3642
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Climb Mill On Vector

Post by TReischl »

Thanks Leo.

Normally what I do is offset the vector by .010 (that is so I can see it easily).

Then I do a quick sketch in Corel showing the vbit with the point on the line like this:
Capture.JPG
And yes, you can make the same sketch in Aspire, I just find it faster in Corel. With a 45 degree chamfer it is really not necessary because the depth of the cut on the offset line is the size of the chamfer plus the offset. With other V bits that does not work.

I do it like that because I do not want the point of the bit running right on the edge of the workpiece, it tends to create a mess. If I have a big enough bit I will offset it even more.

The other thing I try to do is the typical router technique of doing the cross grain cuts first so that it minimizes splintering.
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
rscrawford
Vectric Wizard
Posts: 983
Joined: Mon Jan 17, 2011 6:49 pm
Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408
Location: Wetaskiwin, Alberta
Contact:

Re: Climb Mill On Vector

Post by rscrawford »

Just change the direction of the vector. A vector is just a line with a direction, so you can get the tool to start at the opposite end to cut the opposite direction.
Russell Crawford
http://www.cherryleaf-rustle.com

Post Reply