I have a situation where I want to use a larger cutting tool to clear some flat areas around some v-carving, but this larger bit won't fit in between some of the lines for v-carving, and the v-carve bit won't clear a flat spot. Is there a way to use a smaller clearance tool on the edges of a cut, then clear the larger areas with a larger bit, and finalize the edges with a V-bit?
I should mention that I am cutting hard maple butcher block with router bits on a Leadwell V-25 with a Fanuc 21Mb controller, with the spindle max rpm at 8000 rpm. Probbly not significant for this question but you never know.....
I've attached the V-Carve file with the clearance tool currently set to an 8th-inch end mill, have at it.
Multiple clearance tools
-
- Vectric Apprentice
- Posts: 53
- Joined: Mon May 07, 2007 8:07 am
- Model of CNC Machine: Leadwell V-25 Fanuc 21MB controller
Multiple clearance tools
- Attachments
-
- fillion1.crv
- (138 KiB) Downloaded 171 times
- jimwill2
- Vectric Wizard
- Posts: 612
- Joined: Tue Aug 31, 2010 1:48 am
- Model of CNC Machine: CaMaster Stinger w/recoil, FTC
- Location: Parkville, Missouri
Re: Multiple clearance tools
I downloaded the crv file but the only thing in the file was a bitmap... I'll have to see what you are trying to cut to be able to help. Did you save it before you sent it? Just guessing but, maybe the v-carve tool isn't the right choice. You may need to pocket inside the letters instead. I could be wrong, I'll have to see what how you want to cut it.
Jim Williams
-
- Vectric Apprentice
- Posts: 53
- Joined: Mon May 07, 2007 8:07 am
- Model of CNC Machine: Leadwell V-25 Fanuc 21MB controller
Re: Multiple clearance tools
Let's try this one then:
- Attachments
-
- fillion2.crv
- (868 KiB) Downloaded 180 times
-
- Posts: 25
- Joined: Fri May 21, 2010 5:13 pm
Re: Multiple clearance tools
I developed an idea for re-roughing that I posted on the CNC Zone, but I'll re-post here...
Say you have a v-carve where you have flat areas which the V-bit won't clear, and you have to start with too small a clearance tool to have any shot. Or you're doing raised lettering and have to machine away the field, where the lettering is very intricate, but the field is large enough that a small cutter would take forever to machine.
The way I do this is to "trick" VCarve to do a re-rough toolpath. This works for regular milling, not just v-carving.
So you want to use a V-bit. A 1/16" will get you close enough for V-carving, but clearing a big field is ridiculous. 1/2" will clear the field but leave too much for the v-bit.
What you do is create a pocket toolpath with the 1/16" bit, using the 1/2" bit as the clearance tool. Then make a V-carve toolpath, using the 1/16" bit as the clearance tool. Then simply delete the V-Carve (Pocket) toolpath. Now you have a 1/2" clearance toolpath, a 1/16" re-rough toolpath, and the V-carve toolpath. As you can see, roughing with the 1/2" bit is way faster, than using a 1/8" or even 1/4" bit.
You can even do this as many times as you need, for example start with 1/2", then 1/4", then 1/8", then 1/16"... for large signs with big fields or V-carve signs that have large flat areas this can increase your speed significantly. And moreso if you have ATC.
I've attached a sample file for you to review. I cannot read past version 5.5. Hope this helps!
Say you have a v-carve where you have flat areas which the V-bit won't clear, and you have to start with too small a clearance tool to have any shot. Or you're doing raised lettering and have to machine away the field, where the lettering is very intricate, but the field is large enough that a small cutter would take forever to machine.
The way I do this is to "trick" VCarve to do a re-rough toolpath. This works for regular milling, not just v-carving.
So you want to use a V-bit. A 1/16" will get you close enough for V-carving, but clearing a big field is ridiculous. 1/2" will clear the field but leave too much for the v-bit.
What you do is create a pocket toolpath with the 1/16" bit, using the 1/2" bit as the clearance tool. Then make a V-carve toolpath, using the 1/16" bit as the clearance tool. Then simply delete the V-Carve (Pocket) toolpath. Now you have a 1/2" clearance toolpath, a 1/16" re-rough toolpath, and the V-carve toolpath. As you can see, roughing with the 1/2" bit is way faster, than using a 1/8" or even 1/4" bit.
You can even do this as many times as you need, for example start with 1/2", then 1/4", then 1/8", then 1/16"... for large signs with big fields or V-carve signs that have large flat areas this can increase your speed significantly. And moreso if you have ATC.
I've attached a sample file for you to review. I cannot read past version 5.5. Hope this helps!
- Attachments
-
- Test.crv
- (750 KiB) Downloaded 210 times
-
- Vectric Wizard
- Posts: 4797
- Joined: Thu May 18, 2006 3:24 pm
- Model of CNC Machine: ShopBot
- Location: North Carolina
Re: Multiple clearance tools
Ed,
Take a look at this file and see if the new toolpaths do what you need.
Using the V-Carve toolpath with area clearance tool checked and Flat Depth checked and set to 0.125" would be a better way to go. You can also make a v-bit clear the corners where the end mill won't reach by editing the v-bit and setting the Final Pass Stepover to a very small amount. Remember, you are trying to clear a flat area with a very pointed tool so the stepover must be a very small value. The picture below shows the setting for the example.
Tim
Take a look at this file and see if the new toolpaths do what you need.
Using the V-Carve toolpath with area clearance tool checked and Flat Depth checked and set to 0.125" would be a better way to go. You can also make a v-bit clear the corners where the end mill won't reach by editing the v-bit and setting the Final Pass Stepover to a very small amount. Remember, you are trying to clear a flat area with a very pointed tool so the stepover must be a very small value. The picture below shows the setting for the example.
Tim
- Attachments
-
- fillion2 V2.crv
- (1.34 MiB) Downloaded 187 times
-
- Vectric Apprentice
- Posts: 53
- Joined: Mon May 07, 2007 8:07 am
- Model of CNC Machine: Leadwell V-25 Fanuc 21MB controller
Re: Multiple clearance tools
Thanks, I'm going to need to learn how to do that.
Re: Multiple clearance tools
I'm looking for multiple tool paths clearing.
I have a large area to pocket, so I am using my 1"surfacing bit to start. That bit is way too big to get within ½" of interior object. I want to use a smaller bit for that last ½". Do I setup an end mill in the vcarve option for final step over? Or does it have to be a v-bit used?
I have a large area to pocket, so I am using my 1"surfacing bit to start. That bit is way too big to get within ½" of interior object. I want to use a smaller bit for that last ½". Do I setup an end mill in the vcarve option for final step over? Or does it have to be a v-bit used?
- Adrian
- Vectric Archimage
- Posts: 14544
- Joined: Thu Nov 23, 2006 2:19 pm
- Model of CNC Machine: ShopBot PRS Alpha 96x48
- Location: Surrey, UK
Re: Multiple clearance tools
You've re-activated a 9 year old thread. The method of multiple clearance tools is totally different in the current versions of the software so if people don't spot the dates the first posts in this thread are going to really confuse them.
If you're doing a large pocket you wouldn't use the v-carve toolpath. Use the pocket toolpath with multiple clearance tools instead. That will do what you want.
If you're doing a large pocket you wouldn't use the v-carve toolpath. Use the pocket toolpath with multiple clearance tools instead. That will do what you want.
Re: Multiple clearance tools
Thank You Adrian,
If needed I'll start this question in a new thread.
When using a pocket toolpath with multiple clearance tools,,, doesn't vcarve still go over the entire surface with each smaller tool? That's where I have been unsuccessful. Trying to clear that last half inch against something else I need to use a much smaller bit. The program adds a huge amount of time because it is surfacing the entire project with that small bit. Not just the area closest to my other object.
(if that makes since )
If needed I'll start this question in a new thread.
When using a pocket toolpath with multiple clearance tools,,, doesn't vcarve still go over the entire surface with each smaller tool? That's where I have been unsuccessful. Trying to clear that last half inch against something else I need to use a much smaller bit. The program adds a huge amount of time because it is surfacing the entire project with that small bit. Not just the area closest to my other object.
(if that makes since )
- adze_cnc
- Vectric Wizard
- Posts: 4327
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: Multiple clearance tools
Were you perhaps using the "Raster" clearance strategy with the "Profile Pass" set to none?
EDIT: I didn't see the newly created thread on this matter at: viewtopic.php?f=2&t=38064&sid=244f40401 ... 2aae04ff2e