V Bit carving

This forum is for general discussion about Aspire

V Bit carving

Postby cconway » Fri Oct 05, 2018 5:00 am

I had a 90 deg bit make a carve of some letters. I did not set any flat depth and started the cut .o1 below the surface. The cut took a chunk out of two of the letters. I assume I will need to have it cut a little deeper to correct the problem. The question is how to I have it cut deeper when I don't know what it cut to the first time. Do I have to increase the size of the letters to make it cut a little deeper or is there another way to handle this?

Thanks!
cconway
 
Posts: 27
Joined: Thu May 17, 2018 9:40 pm
Location: Oxford, CT
Model of CNC Machine: Shark HD4 Extended/Water cooled spindle

Re: V Bit carving

Postby Rcnewcomb » Fri Oct 05, 2018 5:21 am

FAQ: How can I adjust the depth of my v-carving when it is too deep or too shallow?

If your v-carving is cutting too deep you have a few options:

Easiest solution is the use the Flat Depth option near the top of the V-Carve / Engraving Toolpath form. This will still cut angled sides using a v-bit but the bottom will be flat and limited to the Flat Depth amount. This can be visibly different than a design carved to full depth without a flat bottom, but may be your only option especially if you need to work with the v-bits you have on hand.

Use a v-bit with a larger included angle, which cuts a shallower v-groove. For example, a 90-degree v-bit will cut shallower than a 60-degree v-bit, and a 120-degree v-bit will cut shallower than a 90-degree v-bit. See eg.1 below for different agnle V-bits on a 2" circle profile.

Reduce the size of the vectors to reduce the gap. Typically not practical once the design is set, but may be one option if you have a limited number of different angle v-bits available.

If your v-carving is cutting too shallow switch to a v-bit with a higher included angle, i.e., more pointed.

Tip: Sometimes you may find the best angled v-bit for your project is one you don't have. Find out what v-bits are commercially available in your area and create tools for them in your tool database. Then use them with the Toolpath Preview until you get the results you want. Now you know exactly which v-bit you need to purchase to complete the project.
Image
- Randall Newcomb
10 fingers in, 10 fingers out - another good day in the shop
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3065
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: V Bit carving

Postby scottp55 » Fri Oct 05, 2018 8:41 am

Depends on how big a "Chunk" of tear out you had.
You could duplicate the toolpath and have a Start Depth of .02" this time. Run the original toolpath preview,then the .02", and see if it would help by comparing against the actual cut without causing any different problems.
Make sure bit is sharp and clean. I usually find tearout can be minimized by reducing Plunge speed and Pass Depth, especially in tiny VCarves.
Another option possible is to sand with a hard pad 80-220G for .01-.02", OR skim your material down in light passes about the same if it gets rid of the tearout, sand to finish grit,applying a coat
of finish often helps. Make sure to remeasure Material and recalculate all toolpaths!
IF material is flat and sanded to finish grit, then the .01" Start Depth shouldn't be necessary.
If deeper depth is required, see Randall's excellent summation above.

IF it's off the spoilboard, all bets are off.
A pic would have helped.
scott
User avatar
scottp55
Vectric Wizard
 
Posts: 2291
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: V Bit carving

Postby cconway » Sat Oct 06, 2018 4:14 pm

My appologies for the delay in responding. I had a personal issue that I had to handle. I appreciate your responses. I have been have a lot of issues with tear out. Her is a picture of what I was referring to.
Attachments
Tear out.jpg
cconway
 
Posts: 27
Joined: Thu May 17, 2018 9:40 pm
Location: Oxford, CT
Model of CNC Machine: Shark HD4 Extended/Water cooled spindle

Re: V Bit carving

Postby martin54 » Sat Oct 06, 2018 5:32 pm

Is that Pine ? If it is or some other softwood then it is always going to want to cause problems with tearout from what I have read, don't do any work with softwoods so no personal experience.
Try slowing your feed rate & reducing your depth of cut, often with text you need to slow things down & reduce the DOC to prevent problems especially with small text :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3904
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: V Bit carving

Postby cconway » Sat Oct 06, 2018 7:16 pm

The wood is soft maple. I appreciate your insight. Thank you.
cconway
 
Posts: 27
Joined: Thu May 17, 2018 9:40 pm
Location: Oxford, CT
Model of CNC Machine: Shark HD4 Extended/Water cooled spindle

Re: V Bit carving

Postby Rcnewcomb » Sat Oct 06, 2018 7:55 pm

For soft maple try first using sanding sealer or shellac before carving. Hard maple carves much better.
- Randall Newcomb
10 fingers in, 10 fingers out - another good day in the shop
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3065
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC

Re: V Bit carving

Postby mtylerfl » Sat Oct 06, 2018 8:40 pm

Do an experiment before cutting future VCarves in Soft Maple (or Pine, for that matter).

I have had near perfect results (no chip out), for both woods by setting rpm at 12,000 and Plunge and Feed Rate at 0.3” per second. No squealing nor burning either. You can try 0.5 ips also, as long as lettering or detail is not too fine and close together (centers of small, lower-case e, o, a, b, etc.).

I generally set the v-bit Pass Depth to 0.25” and run all VCarves twice for super-clean results. (No depth change at all for the second “clean-up” like some folks do. I’ve not found that necessary - just duplicate the original as-is. )
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3222
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: V Bit carving

Postby martin54 » Sat Oct 06, 2018 8:45 pm

Sanding sealer can help as Randall has pointed out, with something like that I might be inclined to apply it twice, lettering might be deeper than the sanding sealer can penetrate so with deeper carvings what I have done in the past is to apply the sanding sealer before I start & then before the final pass of the v bit I stop the cut & apply another coat of sanding sealer to the letters, I use a spirit based shellac sanding sealer which dried very quickly so doesn't add a lot of time to the job :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3904
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: V Bit carving

Postby cconway » Sun Oct 07, 2018 12:54 am

Thank you everyone for sharing your knowledge and insight. Michael I was set at .5 ips so I'll try it at .3 ips on a test run and see how that works. I also get everyone's point on the sanding sealer. I could see where that could help.
cconway
 
Posts: 27
Joined: Thu May 17, 2018 9:40 pm
Location: Oxford, CT
Model of CNC Machine: Shark HD4 Extended/Water cooled spindle

Re: V Bit carving

Postby mtylerfl » Sun Oct 07, 2018 1:18 am

I’ll be interested to read your follow-up post after trying the suggestions. Whenever you have the chance, of course...I know you have a lot of projects going on right now, Charlie!
Michael Tyler

carvebuddy.com

facebook.com/carvebuddy

-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
User avatar
mtylerfl
Vectric Wizard
 
Posts: 3222
Joined: Thu Jan 29, 2009 3:54 am
Location: Brunswick, GA
Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha

Re: V Bit carving

Postby cconway » Sun Oct 07, 2018 2:55 am

I will do that and include pictures.
cconway
 
Posts: 27
Joined: Thu May 17, 2018 9:40 pm
Location: Oxford, CT
Model of CNC Machine: Shark HD4 Extended/Water cooled spindle

Re: V Bit carving

Postby KeithW » Sun Oct 07, 2018 6:31 am

If you are using a True Type font (you didn't specify), why do you set a depth and start below the surface? The machine should cut a font to the proper depth for the bit being used. The V bit will cut to the edge of the font, thereby causing it to be narrow to wide as needed in some fomts.

I don't see any reason to start below the surface level, as that will force it to cut the letters deeper and wider that they are suppose to be, and they will appear to be too close together.

A depth can be set if the letters are BIG as they will want to cut deeper to reach the sides of the font, which will give you a v-carve with a flat bottom.

IF you are using a single line font then a depth will need to be set.

I may have totally missed the issue here, but don't try to second guess the v carve function by 'forcing' some other setting that may not be needed.
KeithW
Vectric Craftsman
 
Posts: 113
Joined: Sun Jun 08, 2014 3:13 am
Location: Red Deer, AB
Model of CNC Machine: Probotix Meteor, Aspire 8.014

Re: V Bit carving

Postby Adrian » Sun Oct 07, 2018 11:10 am

KeithW wrote:If you are using a True Type font (you didn't specify), why do you set a depth and start below the surface? The machine should cut a font to the proper depth for the bit being used. The V bit will cut to the edge of the font, thereby causing it to be narrow to wide as needed in some fomts.

I don't see any reason to start below the surface level, as that will force it to cut the letters deeper and wider that they are suppose to be, and they will appear to be too close together.

I often set a start depth at 1mm below the surface with a v-carving toolpath. I then spray paint the whole piece and plane off the top 1mm which leaves me with clean edged carving and the natural wood everywhere else ready for varnishing. It does distort the letters ever so slightly but at small depths like that it's not noticeable.
User avatar
Adrian
Vectric Archimage
 
Posts: 8421
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: V Bit carving

Postby scottp55 » Sun Oct 07, 2018 11:57 am

Aah...Hadn't even thought about that as I haven't painted yet. Thanks Adrian!

Yep, You have a little chatter there as well, which can really affect tearout.
Your machine may not be as rigid as Michael's, so you may have to reduce your pass depth as well.
Every machine is different as well as species, you'll have to tweak it for yourself to keep the bit cool to the touch, and get the quality of cut you want.

Faster growing trees aren't as dense, and more soft wood between the growth rings for tearout.
In Connecticut you should have Sugar Maple readily available at reasonable cost.
It might be worth your while to check out as cuts are generally much more consistent, and less problems.
Sugar Maple can generally cut and hold detail better also.

I've got a lot of Hard Maple chilren's blocks, and Dad mistakenly ordered soft maple blocks twice...MASSIVE difference in tearout and rejects.
A lot depends on the bit as well.
In Sugar Maple pics of a project I'm doing, with Drillman1's .125" 45 degree 2 flute(all the regular VCarved words)...the speed was IPS .8,.4(plunge),17K and .06" passes.
The Tiny signature font was an Onsrud .25" 30 degree engraving single flute with a .005"flat at .5, .35, 18K.
Both had first coat of Earthpaint Linseed(no dryers)/Beeswax applied first, after sanding to final 600G.

Looking forward to you having good cuts! :)
scott
Attachments
9.5.18 BLOCKS 2.jpg
9.5.18 BLOCKS 4 SIG.jpg
User avatar
scottp55
Vectric Wizard
 
Posts: 2291
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Next

Return to Aspire - General

Who is online

Users browsing this forum: StuC and 27 guests