Climb Mill On Vector
-
- Vectric Craftsman
- Posts: 277
- Joined: Mon Apr 29, 2013 3:37 am
- Model of CNC Machine: Tormach PCNC770
- Location: Cobourg, ON, Canada
Climb Mill On Vector
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?
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?
-
- Vectric Wizard
- Posts: 447
- Joined: Thu Oct 02, 2014 1:49 pm
- Model of CNC Machine: FMT Patriot 4 x8
Re: Climb Mill On Vector
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.
-
- Vectric Craftsman
- Posts: 277
- Joined: Mon Apr 29, 2013 3:37 am
- Model of CNC Machine: Tormach PCNC770
- Location: Cobourg, ON, Canada
Re: Climb Mill On Vector
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.
-
- Vectric Wizard
- Posts: 447
- Joined: Thu Oct 02, 2014 1:49 pm
- Model of CNC Machine: FMT Patriot 4 x8
Re: Climb Mill On Vector
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.
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.
- TReischl
- Vectric Wizard
- Posts: 4642
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: Climb Mill On 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.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).
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 Johns
- Leo
- Vectric Wizard
- Posts: 4086
- 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
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, combined with the functionality of CNC
- TReischl
- Vectric Wizard
- Posts: 4642
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: Climb Mill On Vector
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.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.
Example:
Then if you set it to a bit bigger, like .02 you get:
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 Johns
-
- Vectric Wizard
- Posts: 1592
- Joined: Sun Sep 16, 2007 2:59 pm
- Model of CNC Machine: Custom DIY
- Location: Lake St Clair, MI, USA
- Contact:
Re: Climb Mill On Vector
Just reverse the direction of the vector.
Gerry - http://www.thecncwoodworker.com
- Leo
- Vectric Wizard
- Posts: 4086
- 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
Yes it will work.TReischl wrote: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.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.
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, combined with the functionality of CNC
- Leo
- Vectric Wizard
- Posts: 4086
- 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
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.
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, combined with the functionality of CNC
- TReischl
- Vectric Wizard
- Posts: 4642
- Joined: Thu Jan 18, 2007 6:04 pm
- Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
- Location: Leland NC
Re: Climb Mill On Vector
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:
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.
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:
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 Johns
- rscrawford
- Vectric Wizard
- Posts: 1103
- 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
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
http://www.cherryleaf-rustle.com