Inlay: Never Get it Right

This forum is for general discussion regarding VCarve Pro
Post Reply
CCTDad
Posts: 14
Joined: Thu Aug 15, 2019 8:51 am
Model of CNC Machine: Shapeoko

Inlay: Never Get it Right

Post by CCTDad »

I am having such a hard time getting an inlay to work, and in fact, have never gotten one to work. I've gone through the Zank and Durrant Procedure for Designing and Machining V-Inlay Projects, and watched the Vectric video on the subject, and still a dismal failure. I'm using an up-to-date version 10 of VCarve Pro on a Shapeoko XXL.

The Vectric video at https://youtu.be/l_QoZpI4als, "Tips & Tricks | VCarve Inlays | Vectric" has a V-Carve/Engraving Toolpath graphic at 8:54 that shows:

Inlay Pocket (Female)
Start Depth 0.0
Flat Depth 0.3
V60 0.25
0.125 clearance tool

Inlay (Male)
Start Depth 0.1
Flat Depth 0.2
V60 .25
0.125 clearance tool
_______

My settings in V-Carve/Engraving Toolpath are:

Female
Start Depth 0.0
Flat Depth 0.3
.25 inch V60

Male
Start Depth 0.1
Flat Depth 0.2
.25 downcut clearing
.25 inch V60

I glued it with a lot of Titebond II, left overnight with 30 pounds of cement blocks on it, then cut it off with a Japanese saw. The inlay is 5.75 inches by 4 inches.

What I get is a deep female and a wafer-thin male which doesn't fill the pocket at all (yes, I understand that it's not supposed to go to the bottom). The thickness of the male, inlaid part, ends-up around .07 to .08 inches, and the thickness of the excess that remains on the male backing after cutting it away is about .13 inches, so the entire male is probably .2 or so (I didn't measure it before I glued it in though). The depth of the female pocket is very deep--far deeper than the male part--but of course I can't get in there with the calipers to check. Nonetheless, I'm going to guess it's in the neighborhood of .25, which means it could be .2 or .3. In any case, I'm far from bottoming-out, and clearly the male is not getting into the pocket far enough. I had been running tests with pine on pine but thought the soft stock might be the problem, so for this one the stock is Toon inlaid with Brushbox, just scraps I had laying around. I'm looking to do this inlay with primavera set in monkeypod, that that's about $45 worth of wood and the last of the wood that matches the rest of the piece, so I need to get it right the first time. What am I doing wrong? Photos attached.

I'm no expert but I've been using VCarve and the Shapeoko for 18 months mostly for intricate, decorative carving, and generally have pretty good luck. I just can't ever seem to get inlays to work.

Thanks much.

Dave
Attachments
IMG_2727.JPG
IMG_2728.JPG

Charlie_l
Vectric Apprentice
Posts: 61
Joined: Sat Jun 30, 2012 1:41 am
Model of CNC Machine: CAMaster Stinger II
Location: Wisconsin

Re: Inlay: Never Get it Right

Post by Charlie_l »

In this example I would have expected a start depth of 0.2 and flat of 0.1 for the male inlay part. That would give you an inlay thickness of 0.2 and a gap under it of about a tenth of an inch.

Of course, I am often wrong.

A smaller gap under the inlay works well too.
Aspire, CAMaster Stinger II

ElevationCreations
Vectric Craftsman
Posts: 133
Joined: Thu May 14, 2015 12:29 am
Model of CNC Machine: AVID PRO-Acorn , Shapeoko SO3 XXL & SO3s
Location: Colorado
Contact:

Re: Inlay: Never Get it Right

Post by ElevationCreations »

Dave, which version of Z axis do you have? Belt or HDZ?

Getting V-Inlays to work properly on a Shapeoko takes some finessing to get the pocket and inlay to come out correctly. I had to approach the inlay with additional steps to get consistency and quality.

Following the video settings exactly is beyond the capability of the Shapeoko. The reliable average max DOC is ~.1-.125" on average, expecting anything beyond this with the machine is introducing errors in the work piece. The Shapeoko won't reliably cut the full DOC on the male inlay piece, as the total DOC in the video for the start depth and flat depth is ~.3". With the HDZ you can push for more DOC, but you still have some rigidity limitations with the V Wheels and belts.

What I found works best for my setup is inlay start depth of .19", flat depth of .11" and pocket flat depth of .2". On the inlay do pocket operations close to the start depth so the machine is not taking as much of a cut. It is a different approach but it works within the limitations of the machine.

There are some good threads and instructions here on the process. I would recommend starting out with something basic with scraps until you get the hang of it then work towards something more complex. Don't be afraid to cut your test jobs in half to see how the inlay fits in the pocket and if you are getting errors.

CCTDad
Posts: 14
Joined: Thu Aug 15, 2019 8:51 am
Model of CNC Machine: Shapeoko

Re: Inlay: Never Get it Right

Post by CCTDad »

Thanks so much for the comprehensive replies. Yeah, I've still got belts. I was also wondering whether the fact that the inlay has such irregular, detailed margins has any effect on the cuts, but in any case, the .07 thick male inlays were really disheartening. Again, I appreciate the help and will give it another shot next weekend keeping in mind what both of you said.

User avatar
Tex_Lawrence
Vectric Craftsman
Posts: 199
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko 3 XXL; V-Carve DT 10.509
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: Inlay: Never Get it Right

Post by Tex_Lawrence »

Dave, I've cut a bit of plastic-to-wood inlays with both 60 and 90 bits. The one thing I learned real quick is to set the "pass depth" in Cutting Parameters to something about 1/3 of the total DOC for the inlay.

My Shapeoko XXL doesn't like the way that Vectric Vcarve Desktop plunges to the max depth when vcarving. That move tests the workholding on the part being cut.
Crooked Wood Products - Custom Wood
Truth lies dormant in our future history ― Tex LXVIII

User avatar
martin54
Vectric Wizard
Posts: 5185
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber System 48,Denford Triac Modified
Location: Crossgates, Scotland

Re: Inlay: Never Get it Right

Post by martin54 »

Not having any experience with your machine it's difficult to comment but ElevationCreations points out some of the weaknesses with the machine, doesn't mean your machine can't do this job it just means you need to think a bit more carefully about your speed, feed & DOC settings.
I would make a couple of small test files & machine those from the same piece of material using different speed, feed & DOC settings, keep notes on what you are doing so you can look back at what you have done with each :lol: :lol:

User avatar
mfirlott
Vectric Craftsman
Posts: 248
Joined: Thu Feb 07, 2013 12:49 am
Model of CNC Machine: Stinger 1 (2014)
Location: Cantley, Quebec, Canada
Contact:

Re: Inlay: Never Get it Right

Post by mfirlott »

I see you mention:
Male
Start Depth 0.1
Flat Depth 0.2

From my notes for when I do the v-inlays, mine are reversed...
Male
Start Depth 0.2
Flat Depth 0.1

Female numbers are the same for me.

Maybe that's the issue.
(Mitch)
CAMaster Stinger I
Vectric Aspire
Epilog 45watt Helix Laser

laflippin
Vectric Craftsman
Posts: 153
Joined: Tue Jun 12, 2018 3:07 pm
Model of CNC Machine: Axiom AR 8 Pro+
Location: Cambria, CA

Re: Inlay: Never Get it Right

Post by laflippin »

Actually, for the Zank Inlay approach, your start and flat depth settings for the male piece are exactly the reverse of what they should be. It may not be intuitive without going through the appropriate diagrams; however, the flat depth used for the male piece defines the gap between the top surface of the female piece and the beginning of the waste material. The male start depth defines how deep the inlay piece will fit into the female carving. The difference between the female flat depth (0.3" in your example) and the male start depth (0.1" in your example) defines the "glue gap"--the interstitial space between male and female pieces. So, you most likely wound up with a glue gap of 0.2" and an inlay depth of only 0.1".

As FixitMike and others have pointed out in the past, the original Zank settings lead to an excessive glue gap--you don't need a 0.1" gap (much less a 0.2" gap!.

The settings I would use for your project are: Female engraving: start depth = 0, flat depth = 0.25". Male carving: start depth = 0.15", flat depth = 0.1". This will give you a 0.1" gap between the female surface and the waste material and a 0.05" glue gap (which is more than enough) and a 0.15" deep inlay.

(Note added: While I was typing out the information above, Mitch also posted the correct answer a few minutes ahead of mine. )

User avatar
FixitMike
Vectric Wizard
Posts: 1710
Joined: Sun Apr 17, 2011 5:21 am
Model of CNC Machine: Shark Pro Plus (retired)
Location: Burien, WA USA

Re: Inlay: Never Get it Right

Post by FixitMike »

Repeat post of my picture of how the settings work.
VCarve Inlay.png
Good judgement comes from experience.
Experience comes from bad judgement.

CCTDad
Posts: 14
Joined: Thu Aug 15, 2019 8:51 am
Model of CNC Machine: Shapeoko

Re: Inlay: Never Get it Right

Post by CCTDad »

This is great you guys. I can't wait for next weekend to do some experimenting.

CCTDad
Posts: 14
Joined: Thu Aug 15, 2019 8:51 am
Model of CNC Machine: Shapeoko

Re: Inlay: Never Get it Right

Post by CCTDad »

Update! See below for a successful .75 inch wide inlay, brush box in pine. I used laflippin's female engraving: start depth = 0, flat depth = 0.25". Male carving: start depth = 0.15", flat depth = 0.1. I wasn't happy with it the first time out, so I slowed down the feed and plunge and went with a 1% stepover and had great success. Now for trying the entire turtle again.

Thanks much everybody.

Dave
.75 inch brush box pine inlay.jpg

Charlie_l
Vectric Apprentice
Posts: 61
Joined: Sat Jun 30, 2012 1:41 am
Model of CNC Machine: CAMaster Stinger II
Location: Wisconsin

Re: Inlay: Never Get it Right

Post by Charlie_l »

As you experiment try male start depth of 0.2 and 0.05 flat depth.

Glad you have it working.
Aspire, CAMaster Stinger II

laflippin
Vectric Craftsman
Posts: 153
Joined: Tue Jun 12, 2018 3:07 pm
Model of CNC Machine: Axiom AR 8 Pro+
Location: Cambria, CA

Re: Inlay: Never Get it Right

Post by laflippin »

Oh gosh! Thank you, Charlie, for suggesting female flat depth of 0.2" ! That is in fact the actual female flat depth that I had meant to suggest (in combination with the male st. depth = 0.15 and male flat depth = 0.1) but I mistakenly typed in 0.25" instead.

I'm glad the project worked out anyway, but using my original numbers did give you a larger glue-gap (0.1") than you need.

So, in future, try what I meant not what I said.... :roll: :lol:

Post Reply