Visiting 3D carving

This forum is for general discussion regarding VCarve Pro

Re: Visiting 3D carving

Postby Xxray » Sat Nov 16, 2019 8:09 pm

BTW, for those who perhaps may think I am on about nothing, 3D finish passes typically take hours, sometimes half a day or more depending on size of the project, bit used and stepover. So those who go this route will just about double their cutting time. Thats Ok by me if thats what you want to do, being a curious guy I would just like to know why.
Doug
User avatar
Xxray
Vectric Wizard
 
Posts: 1967
Joined: Thu Feb 17, 2011 8:47 am
Location: MI USA
Model of CNC Machine: CAMaster Stinger 1

Re: Visiting 3D carving

Postby martin54 » Sat Nov 16, 2019 9:21 pm

BigC wrote:Forgoing if the second roughing pass is necessary or not and just go ahead with perhaps a smaller roughing bit and then use the tapered ball mill.
A question about the tapered ball mill if I may please,
How exactly would I go about setting one of these up (Tapered Ball Mill) in the Tool Database? (*typical newbie question :oops: )
and are they a useful bit to have to hand.
I may add one of these bits to my Santa List
Tool Database clip.JPG

Many Thanks
Regards
C


Set up as has already been said, things like side angle is normally info provided by the manufacturer.

As for are they a useful tool, well if you are doing 3D work then I would say yes they are very useful, with some of the 3D stuff I carve I would say they are essential, a small diameter ball nose is so fragile when cutting hardwoods, I have a few different sizes from 0.5mm to 4mm diameter. If your adding to your santa list then you might want to add a couple. Really depends on what sort of thing you are cutting & what size :lol: :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 4663
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Visiting 3D carving

Postby BigC » Sun Nov 17, 2019 7:39 am

Adrian
Adrian wrote:There is a tapered ball nose tool type in the list of tools. Click the Add Tool icon in the bottom left and then choose the Tapered Ball Nose from the dropdown that appears in the dialog.

I see that now
Many Thanks, Adrian
Regards
C
tBN.JPG


Martin54
Set up as has already been said, things like side angle is normally info provided by the manufacturer.
As for are they a useful tool, well if you are doing 3D work then I would say yes they are very useful, with some of the 3D stuff I carve I would say they are essential, a small diameter ball nose is so fragile when cutting hardwoods, I have a few different sizes from 0.5mm to 4mm diameter. If your adding to your santa list then you might want to add a couple. Really depends on what sort of thing you are cutting & what size :lol: :lol: :lol:

Thanks for your reply Martin
"TWO," you say :lol: Hmmmm ..As I mainly cut Pine, Oak, Plywood, and MDF at the moment because they are the most accessible for a newbie to get his hands upon what sizes would you suggest for the two that I should buy to cut Pine and Oak 25mm thick or less (cough:: put on the list).
As a newcomer to the hobby side of things I already have ordinary straight BN bits mainly 3 and 6mm so maybe a 0.5 and a 1 or 2mm tBN perhaps?
Please advise
Apologies to the OP for cutting across his thread
Regards
C
BigC
Vectric Craftsman
 
Posts: 208
Joined: Tue Apr 02, 2019 7:06 pm
Model of CNC Machine: Workbee

Re: Visiting 3D carving

Postby Jan.vanderlinden » Sun Nov 17, 2019 6:46 pm

Interesting thoughts and comments here, and I appreciate all of them.
I tried using this process in an effort to get cleaner detail and less wear on the tapered end mill.
I used to do the roughing pass and then go directly to the TBEM
In doing so, I was experiencing greater tool wear and the detail was not as clean due to cutter deflection of the TBEM and or fuzzies
But coming from a tool & die background, we always used and roughing pass, simi finish pass, and then a finial finish pass.
So I thought, why not try it.
When I go to the finial finish pass with the TBEM I may or may not drop the Z ~.005" ( depending on how the simi finish cut looks)
Yes, we are all looking for a faster way to do our machining, and this definitely takes more machine time.
The upside is a more detailed and cleaner (fuzzies) carving, and minimal hand sanding.
For me the extra machine time is worth it and It's now my new process.

In the above deer scene
My roughing pass is with a .25" EM, .06" depth of cut, .06" step over and 100 IPM, Z level
My simi finish pass is with a .25" BEM, .025" step over, 100 IPM, Raster at 45°
My finish pass is with a 4.8° .02" Dia. TBEM .005" step over 100 IPM Raster at 0°
I've learned so much from my mistakes, I'm thinking of making a few more.
Jan.vanderlinden
Vectric Craftsman
 
Posts: 202
Joined: Wed Sep 28, 2016 10:19 pm
Location: Columbus Ohio
Model of CNC Machine: Xcarve

Re: Visiting 3D carving

Postby rscrawford » Sun Nov 17, 2019 8:51 pm

Jan.vanderlinden wrote:Interesting thoughts and comments here, and I appreciate all of them.
I tried using this process in an effort to get cleaner detail and less wear on the tapered end mill.
I used to do the roughing pass and then go directly to the TBEM
In doing so, I was experiencing greater tool wear and the detail was not as clean due to cutter deflection of the TBEM and or fuzzies
But coming from a tool & die background, we always used and roughing pass, simi finish pass, and then a finial finish pass.
So I thought, why not try it.
When I go to the finial finish pass with the TBEM I may or may not drop the Z ~.005" ( depending on how the simi finish cut looks)
Yes, we are all looking for a faster way to do our machining, and this definitely takes more machine time.
The upside is a more detailed and cleaner (fuzzies) carving, and minimal hand sanding.
For me the extra machine time is worth it and It's now my new process.

In the above deer scene
My roughing pass is with a .25" EM, .06" depth of cut, .06" step over and 100 IPM, Z level
My simi finish pass is with a .25" BEM, .025" step over, 100 IPM, Raster at 45°
My finish pass is with a 4.8° .02" Dia. TBEM .005" step over 100 IPM Raster at 0°



You won't get less wear on your tapered bullnose by using this double finish tool path method. You are still getting wear on the very tip of the tapered ballnose, which is the area you want to remain the sharpest. The rest of the cutter, which you never use anyway, will remain sharp but that is useless anyway when you cut like this since you only ever use the very tip. Cutting wood is VERY different than cutting steel. Often we need to do the exact opposite of what makes sense in milling steel.

If you want to get the least wear on your cutters, you want to be removing enough of a chip size so that you actually cutting instead of simply 'burnishing' the edge. For maximum cutter longevity, you would go straight to a single finish tool path with a tapered ballnose cutter and skip the roughing pass and the first finish tool path.

Now, most people will tell you that skipping the roughing tool path is hard on your tools. But think about what you are actually doing. With a 1/16" tip on a tapered ballnose, at 8% stepover, you are only cutting 0.005" per pass. This does not put any stress on your ballnose, or your machine, even if you are cutting to a depth of 1". The first pass is the only pass that is putting stress on your cutter, so you may want to slow down the first pass, then speed back up for the rest.

What the roughing tool path does (and this is important for some projects) is remove the stresses from your wood before the finish toolpath. It also removes extra material that may get in the way of a short cutting edge on your finish tool path tool, which usually isn't a problem with the tapered ballnose bits because they usually have longer cutter lengths.
Russell Crawford
http://www.cherryleaf-rustle.com
User avatar
rscrawford
Vectric Wizard
 
Posts: 951
Joined: Mon Jan 17, 2011 6:49 pm
Location: Wetaskiwin, Alberta
Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408

Re: Visiting 3D carving

Postby BigC » Sun Nov 17, 2019 9:52 pm

In the above deer scene
My roughing pass is with a .25" EM, .06" depth of cut, .06" step over and 100 IPM, Z level
My simi finish pass is with a .25" BEM, .025" step over, 100 IPM, Raster at 45°
My finish pass is with a 4.8° .02" Dia. TBEM .005" step over 100 IPM Raster at 0°

From a newbie standpoint, is it essential that you run a roughing pass as a Z level and the two finishing passes as rasterized?
Regards
C
BigC
Vectric Craftsman
 
Posts: 208
Joined: Tue Apr 02, 2019 7:06 pm
Model of CNC Machine: Workbee

Re: Visiting 3D carving

Postby Xxray » Sun Nov 17, 2019 10:34 pm

Jan.vanderlinden wrote:Interesting thoughts and comments here, and I appreciate all of them.
I tried using this process in an effort to get cleaner detail and less wear on the tapered end mill.
I used to do the roughing pass and then go directly to the TBEM
In doing so, I was experiencing greater tool wear and the detail was not as clean due to cutter deflection of the TBEM and or fuzzies
But coming from a tool & die background, we always used and roughing pass, simi finish pass, and then a finial finish pass.
So I thought, why not try it.
When I go to the finial finish pass with the TBEM I may or may not drop the Z ~.005" ( depending on how the simi finish cut looks)
Yes, we are all looking for a faster way to do our machining, and this definitely takes more machine time.
The upside is a more detailed and cleaner (fuzzies) carving, and minimal hand sanding.
For me the extra machine time is worth it and It's now my new process.

In the above deer scene
My roughing pass is with a .25" EM, .06" depth of cut, .06" step over and 100 IPM, Z level
My simi finish pass is with a .25" BEM, .025" step over, 100 IPM, Raster at 45°
My finish pass is with a 4.8° .02" Dia. TBEM .005" step over 100 IPM Raster at 0°


Thanks for the insight Jan. I don't want to belabor the point but there is still no technical reason why your method would yield anything other than wasted time. Have you ever done identical projects back to back, one with the extra pass and one without, to validate the claim that you are getting a more precise, cleaner cut ? You can't really gauge bit wear without some very precise measuring tools and even then, it is doubtful that a single project, or even a few, would show any difference at all in bit wear. Best ways to tell if you are pushing past bit capabilities is if you are creating dust and/or smoke. If you aren't then chances are that you don't need to try to fix something that isn't broken. If you are having deflection issues it very likely may be a non rigid machine issue rather than cutting strategy.
But by all means, keep at it, pleasing yourself is all that matters in this racket and I don't mean to be an ass by being critical of your method. I really just wanted to add some perspective for those with less experience like the OP who might copy your method then get frustrated that cuts take hours and hours and hours more than they had thought.
Doug
User avatar
Xxray
Vectric Wizard
 
Posts: 1967
Joined: Thu Feb 17, 2011 8:47 am
Location: MI USA
Model of CNC Machine: CAMaster Stinger 1

Previous

Return to VCarve - General

Who is online

Users browsing this forum: No registered users and 31 guests