A simple way to make inlays

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro

Re: A simple way to make inlays

Postby jhanna » Fri Jun 01, 2018 3:23 am

I echo Tim's question which doesn't seem to have been answered... I'm trying to make an inlay that is 0.25" deep. For the female pocket I used a start depth of 0 and a flat depth of 0.25". For the male plug I used a start depth of 0.24" and a flat depth of 0.1". Even though my flat area clearance tool has a pass depth of 0.1", it takes the full 0.34" depth in one pass. What am I missing?

tvannaman2000 wrote:My concern is with the starting depth of the male part of the inlay. I'm using a clearing bit (1/8" or 1/16") to remove a lot of the material first before I use the vbit and that first cut is too deep because of the start depth setting. Once that first pass is done, the remaining passes are fine. ie. I want to cut no more than .05" per pass but if my starting depth is already .05, it will try to cut .1 on the first pass. I guess I could go in and adjust my pass info, but if the starting depth is larger than your max depth setting for the bit, you risk breaking bits or munging wood. How do you people handle that?
Tim.
jhanna
 
Posts: 5
Joined: Mon Apr 23, 2018 5:20 pm
Model of CNC Machine: Shapeoko 3 XL

Re: A simple way to make inlays

Postby Adrian » Fri Jun 01, 2018 11:37 am

jhanna wrote:I echo Tim's question which doesn't seem to have been answered... I'm trying to make an inlay that is 0.25" deep. For the female pocket I used a start depth of 0 and a flat depth of 0.25". For the male plug I used a start depth of 0.24" and a flat depth of 0.1". Even though my flat area clearance tool has a pass depth of 0.1", it takes the full 0.34" depth in one pass. What am I missing?


You're missing that there shouldn't be any material above the start depth when the toolpath is used for the purposes it was designed for so the pass is actually 0.1". The 0.24" part doesn't count as it should be empty space.
User avatar
Adrian
Vectric Archimage
 
Posts: 9594
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: A simple way to make inlays

Postby adze_cnc » Fri Jun 01, 2018 5:04 pm

As far as Tim's question if he's snapping an 1/8" cutter when it's cutting only cutting 0.1" deep I suspect his feeds and speeds are far too aggressive for his machine and the cutter.

I recently cut some beech using a single-flute 1/8" cutter with 1/8" shank and 3/4" cutting edge length at 18,000 rpm and 75" per minute and a pass depth of 1/8" and had no problems---I could have even gone faster or even taken a deeper cut.

Having said that, my spindle is 5hp and my machine is quite rigid so I have a certain advantage against flex and breakage.
User avatar
adze_cnc
Vectric Apprentice
 
Posts: 719
Joined: Sat Jul 27, 2013 10:08 pm
Location: Vancouver, BC, Canada
Model of CNC Machine: AXYZ 4008

Re: A simple way to make inlays

Postby jhanna » Fri Jun 01, 2018 6:52 pm

Adrian wrote:You're missing that there shouldn't be any material above the start depth when the toolpath is used for the purposes it was designed for so the pass is actually 0.1". The 0.24" part doesn't count as it should be empty space.


Understood. Is there a better way to deal with this other than setting the Z zero above the surface and running multiple clearing passes with your own pass depth manually controlled by Z zero?

Thanks
Jeff
jhanna
 
Posts: 5
Joined: Mon Apr 23, 2018 5:20 pm
Model of CNC Machine: Shapeoko 3 XL

Re: A simple way to make inlays

Postby Samson » Sat Jun 02, 2018 12:08 am

jhanna wrote:I echo Tim's question which doesn't seem to have been answered... I'm trying to make an inlay that is 0.25" deep. For the female pocket I used a start depth of 0 and a flat depth of 0.25". For the male plug I used a start depth of 0.24" and a flat depth of 0.1". Even though my flat area clearance tool has a pass depth of 0.1", it takes the full 0.34" depth in one pass. What am I missing?



If I read this correctly, you have your numbers inverted. Should be start depth of .1", and flat depth of .24".
Samson
Vectric Wizard
 
Posts: 301
Joined: Fri May 02, 2014 10:14 pm
Model of CNC Machine: 4x4

Re: A simple way to make inlays

Postby tvannaman2000 » Sun Jul 29, 2018 5:02 am

I'm running a DeWalt router on an X-Carve so while I have the upgraded single X axis bar, it's not the stiffest machine around. I'd typically run a 1/8" bit around 40ipm on most woods with a .04" doc. If it's oak, I back it off to .02" doc to prevent losing steps and burning wood. For some of my clearing cuts, if I back off the speed to account for the first deep pass, it takes about 10x time to finish the rest of the carve at "normal" depth of cuts.
tvannaman2000
Vectric Apprentice
 
Posts: 18
Joined: Fri Oct 07, 2016 2:49 am
Model of CNC Machine: X-Carve

Re: A simple way to make inlays

Postby FixitMike » Sun Jul 29, 2018 7:35 am

jhanna wrote:I echo Tim's question which doesn't seem to have been answered... I'm trying to make an inlay that is 0.25" deep. For the female pocket I used a start depth of 0 and a flat depth of 0.25". For the male plug I used a start depth of 0.24" and a flat depth of 0.1". Even though my flat area clearance tool has a pass depth of 0.1", it takes the full 0.34" depth in one pass. What am I missing?


The first pass will be at the start depth plus the tool pass depth or flat depth if it is less. The toolpaths assume that the material to be cut starts at the start depth. This is usually true since the start depth is usually used when you are making a cut in a pocket that has already been cut. I don't know of a way around this.
Good judgement comes from experience.
Experience comes from bad judgement.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1542
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (extensively modified)

Re: A simple way to make inlays

Postby meflick » Thu Mar 21, 2019 4:04 pm

Thank you for sharing your directions and for the long "life" of this thread.

Beki made a presentation on this at the Chicago Users Group meeting and Vectric has now shared that presentation and a free project to try. You can find the link and information on it here:
http://forum.vectric.com/viewtopic.php? ... ead#unread

Thank you to Beki for doing that and to Vectric for sharing it. Thank you to all forum users who have continued to provide insight and help on this thread as well. I hope to give it a try soon.
User avatar
meflick
Vectric Apprentice
 
Posts: 67
Joined: Tue Dec 05, 2017 3:41 pm
Location: East TN - USA
Model of CNC Machine: Shark HD4

Re: A simple way to make inlays

Postby laflippin » Mon Oct 07, 2019 11:53 pm

The importance of experimenting with feed rate and pass depth....DOH!

I'm almost sure that my recent experience is a simple echo of learning that has already been recorded in here somewhere but, here goes:

Have been cutting 1"x 9" x 14" oval trays out of 1.5 x 11.75 x 16 stock (Douglas fir). Then, V-engraving various images on the floor of the trays, V-carving the male mirror image pieces for Zank inlay, and so on.

Problem: Using a 1/2" 60 deg V-bit at the default values (0.2in pass depth; 100 ipm feed rate) I was getting really unacceptable chipping in some delicate but important areas of both female and male workpieces (see, for example, female engravings 1 & 1a, below).

Solution: Changed two variables that I thought might be contributing to the problem. (1) Decreased the V-bit pass depth to 0.1in [Note: At my start depth (.15) and flat depth (.1) numbers for the male pieces the pass depth change was of no consequence. However, the females were flat depth = 0.2 in, and so the new 0.1" pass depth looked a lot less stressful on the delicate engraving details. (2) Decreased the feed rate to 80 ipm.

Hard to know the %-contributions of these two independent variables in the female engravings, but the results are so nice....I'm not going back right now to sort that out. But, though unfortunately I don't have both "before-and-after" pix for a male piece, I do have an 80 ipm example (i.e., the "after" piece; some delicate twigs in walnut)--wow! Lowering the feed rate alone, by only 20%, made a big, big difference---much cleaner, no chipping, hardly any "fuzzies"--the picture below is hot off the CNC, none of the usual clean-up with tweezers/picks/brushes.
female engraving1; 0.2in pass depth; 100 ipm.JPG
female engraving 1; 0.2in pass depth; 100 ipm feed rate
female engraving1a; 0.1in pass depth; 80 ipm.JPG
female engraving 1a; 0.1in pass depth; 80 ipm feed rate
male carving; walnut; 80 ipm.JPG
male carving; walnut; 80 ipm
laflippin
Vectric Craftsman
 
Posts: 102
Joined: Tue Jun 12, 2018 3:07 pm
Location: Cambria, CA
Model of CNC Machine: Piranha FX, Axiom AR 8 Pro+

Re: A simple way to make inlays

Postby rtibbs2018 » Wed Oct 09, 2019 11:05 pm

I know I'm coming late to this thread however I'm just starting some inlay projects and I found this on YouTube.
The link is as follows:

https://www.youtube.com/watch?v=l4VMo9DCzO8

If it's been posted already I apologize. I did scan through the 24 pgs. of this thread and didn't find a reference to it.
Of course, I could have missed the forest for the trees. :oops:
rtibbs2018
Vectric Craftsman
 
Posts: 114
Joined: Mon Nov 12, 2018 11:15 pm
Location: Central Florida
Model of CNC Machine: Shopbot desktop

Re: A simple way to make inlays

Postby laflippin » Fri Oct 11, 2019 8:02 pm

rtibbs,

Shawn Gano is a very smart guy (actually a NASA engineer) who indulges in many fascinating personal hobbies including various Zank V-carve Inlay projects. He learned the basic techniques of Zank's inlay procedures from the 2006 white paper that Paul posted here, and probably also picked up quite a bit more from the many posts to this thread that followed the Zank white paper. I corresponded with him about the history of the Zank inlay technique and, although he unfortunately doesn't seem to have posted anything here, he did say that he included a citation to the Zank white paper in his YouTube video. That said, his video is really a very nice addition to the mix of instructional materials on the technique--for example, it is much more interesting and instructive than another YouTube video (unnamed here) featuring a guy who happily admits that he just plugs in start depth and flat depth numbers by imitation and has no idea what they mean.

Coming from a professional background in which it is considered very important to properly cite the foundational work of others, I do find it disappointing that (with a few notable exceptions) many folks who enjoy the power and beauty of Zank V-carve Inlay in their work don't always bother to overtly give credit where it is due. As I've said before in threads here at Vectric, there are at least two good reasons to refer to your inlay projects accomplished with Vectric's V-carve toolpaths as "Zank V-carve Inlay Protocols" or Zank VIP, or at least Zank inlay: (1) It assigns proper credit to the actual inventor and, (2) It importantly differentiates this powerful inlay technique from Vectric's canned Inlay toolpaths, which have little, if any, relation to Zank V-carve inlay. There have been numerous occasions in which people have needlessly confused these two very different techniques.
inlaid oval tray.JPG
laflippin
Vectric Craftsman
 
Posts: 102
Joined: Tue Jun 12, 2018 3:07 pm
Location: Cambria, CA
Model of CNC Machine: Piranha FX, Axiom AR 8 Pro+

Previous

Return to VCarve - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 4 guests