VCarve inlays and flat depth

This forum is for general discussion regarding VCarve Pro

Re: VCarve inlays and flat depth

Postby edwardharp » Mon Jun 11, 2018 8:05 pm

scottp55 wrote:Not seeing why VCarving with an engraving bit isn't working...been doing it for quite some time(and as recently as today with a .025"flat).
Using VCP9 now...but it worked in 8.
scott


I am going to have to try it again. Maybe they fixed it in intervening versions? Last I tried it was at least two years ago I would say.

I mostly work in wood these days and those cutters don't have a flat depth.

Thanks!
edwardharp
Vectric Apprentice
 
Posts: 19
Joined: Tue May 29, 2018 3:19 am
Model of CNC Machine: Tormach PCNC 1100

Re: VCarve inlays and flat depth

Postby edwardharp » Mon Jun 11, 2018 8:08 pm

ger21 wrote:
edwardharp wrote:It all depends on the size of the inlays, the grain of the wood, the species of the wood, etc. And the limitations of the machine for that matter. I use a CNC milling machine because I also do metal and other materials and there is a limit to how fast I can spin the V cutter.


Can you mount an auxiliary high speed spindle to your machine?
That's really the problem here. With a high speed spindle, you probably wouldn't be having the issues that you are.


I can actually. There are a few options. And I am thinking about upgrading my machine to one that is 50% faster.

Considering how many of these inlays I am doing I should at least try a companion spindle. Those can do 20,000 RPM. But ugh are they loud!

The worst problem will be that changing tools will mean different offsets. I wont be able to mount end mills on the companion spindle. There is also a water cooled main spindle but it would interfere with my metal work.

Good suggestion though. Thanks.
edwardharp
Vectric Apprentice
 
Posts: 19
Joined: Tue May 29, 2018 3:19 am
Model of CNC Machine: Tormach PCNC 1100

Re: VCarve inlays and flat depth

Postby edwardharp » Mon Jun 11, 2018 8:19 pm

ger21 wrote:
edwardharp wrote:It all depends on the size of the inlays, the grain of the wood, the species of the wood, etc. And the limitations of the machine for that matter. I use a CNC milling machine because I also do metal and other materials and there is a limit to how fast I can spin the V cutter.


Can you mount an auxiliary high speed spindle to your machine?
That's really the problem here. With a high speed spindle, you probably wouldn't be having the issues that you are.


Any idea how fast a spindle I would need? Would 10,000 RPM be fast enough?
edwardharp
Vectric Apprentice
 
Posts: 19
Joined: Tue May 29, 2018 3:19 am
Model of CNC Machine: Tormach PCNC 1100

Re: VCarve inlays and flat depth

Postby BDM » Tue Jun 12, 2018 1:50 pm

edwardharp wrote:
I can actually. There are a few options. And I am thinking about upgrading my machine to one that is 50% faster.

Considering how many of these inlays I am doing I should at least try a companion spindle. Those can do 20,000 RPM. But ugh are they loud!

The worst problem will be that changing tools will mean different offsets. I wont be able to mount end mills on the companion spindle. There is also a water cooled main spindle but it would interfere with my metal work.

Good suggestion though. Thanks.


I don't have a vast experience with different spindles, but they certainly don't have to be loud. The air cooled one our school has is so quiet that the first time I used it, I had to look closely at the collet to see that it actually was spinning. Why wouldn't you be able to use an end mill on a companion spindle?
BDM
Vectric Craftsman
 
Posts: 122
Joined: Tue Jan 04, 2011 3:52 pm
Location: S.E. Michigan

Re: VCarve inlays and flat depth

Postby Adrian » Tue Jun 12, 2018 2:41 pm

My spindle runs at up to 18000 rpm and you can have a normal conversation right by it at that speed. If it's really loud I expect it's a router masquerading as a spindle. ;)
User avatar
Adrian
Vectric Archimage
 
Posts: 8606
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: VCarve inlays and flat depth

Postby edwardharp » Mon Jul 02, 2018 6:31 am

I ended up trying a Kress companion spindle capable of 29,000 RPM. Reasonably quiet.

First few attempts did not turn out as well as I hoped. I will try messing with feeds and see if I can coax it into behave better.

I am also crunching away at how all this works and how I might accomplish this without the start depth thing so that I can control cut depth.
edwardharp
Vectric Apprentice
 
Posts: 19
Joined: Tue May 29, 2018 3:19 am
Model of CNC Machine: Tormach PCNC 1100

Re: VCarve inlays and flat depth

Postby potzmannwoodshop » Mon Jul 02, 2018 5:56 pm

Adrian wrote:My spindle runs at up to 18000 rpm and you can have a normal conversation right by it at that speed. If it's really loud I expect it's a router masquerading as a spindle. ;)


Mine turns at 18k too, and a conversation isnt easy while is it running. 3phase 10hp Air Cooled Industrial spindle with Yaskawa drives.
potzmannwoodshop
Vectric Apprentice
 
Posts: 80
Joined: Wed Feb 15, 2017 2:03 pm
Model of CNC Machine: 2 SCM Routech Record 120s(1999, 2001)

Re: VCarve inlays and flat depth

Postby Woodwasp » Tue Jul 03, 2018 5:37 am

My way of handling this issue is to write 2 tool paths for the male inlay one with a shallow cut to remove the bulk above the start depth, then a second cut at the start depth which removes only a small amount of material. Save both tool paths in the one file being very careful to get them in the right order. When you send the g-code to your machine it will cut one after the other, Yes this take a little longer but we are striving for successful fine detail not speed. I find this method tends to eliminate chip out and results in fine inlay detail.
Woodwasp
 
Posts: 3
Joined: Sun Jan 31, 2016 5:34 am
Model of CNC Machine: Xcarve

Re: VCarve inlays and flat depth

Postby SCG » Fri Aug 10, 2018 10:14 pm

So, I've tried repeatedly to implement the use of vcarve feature, pocket, mirrored male inlay plug for vcarve inlays. I've followed every instructional resource available with no success. The mirrored "male plug" is always too deep and too loose for a proper fit. I've used the .2 flat depth for Pocket and .1 start depth, .1 flat depth for mirrored male inlay plug. It's wrong and never works. At least this is the case for VCP 9. My only" almost successful" successful v inlay was .15 pocket flat depth , .075 start depth and .075 flat depth on reversed male plug. It was very sloppy with way too much gap between the pocket and inlay piece. May have worked in VCP 8 but not in VCP 9. I no longer try to use this method.
SCG
 
Posts: 6
Joined: Thu Jul 26, 2018 8:02 am
Model of CNC Machine: Axiom AR8 Pro

Re: VCarve inlays and flat depth

Postby FixitMike » Sat Aug 11, 2018 1:59 am

SCG wrote:So, I've tried repeatedly to implement the use of vcarve feature, pocket, mirrored male inlay plug for vcarve inlays. I've followed every instructional resource available with no success. The mirrored "male plug" is always too deep and too loose for a proper fit. I've used the .2 flat depth for Pocket and .1 start depth, .1 flat depth for mirrored male inlay plug. It's wrong and never works. At least this is the case for VCP 9. My only" almost successful" successful v inlay was .15 pocket flat depth , .075 start depth and .075 flat depth on reversed male plug. It was very sloppy with way too much gap between the pocket and inlay piece. May have worked in VCP 8 but not in VCP 9. I no longer try to use this method.


1. The flat depth on the male plug sets the gap.
2. The start depth of the male plug determines how far the plug extends into female. I make it .02" to .04" less than the flat depth of the female.. The instructions, in my opinion, don't sink the male plug far enough into the female.
3. When properly cut, the two pieces will almost lock in place.
4 Be sure to use the same V bit on both parts, and be sure its angle is what you have specified for the tool. I used the wrong angle bit once and the pieces did not fit together very well.

And a hint: Apply a coat or 2 of finish to the female material before cutting. It will make it easier to clean up the glue squeeze out. And be sure to clean up both pieces before putting them together. I use a dental pick to remove any tiny unwanted pieces.
Good judgement comes from experience.
Experience comes from bad judgement.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1451
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (modified)

Re: VCarve inlays and flat depth

Postby LittleGreyMan » Sat Aug 11, 2018 9:59 am

SCG wrote:So, I've tried repeatedly to implement the use of vcarve feature, pocket, mirrored male inlay plug for vcarve inlays. I've followed every instructional resource available with no success. The mirrored "male plug" is always too deep and too loose for a proper fit. I've used the .2 flat depth for Pocket and .1 start depth, .1 flat depth for mirrored male inlay plug. It's wrong and never works. At least this is the case for VCP 9. My only" almost successful" successful v inlay was .15 pocket flat depth , .075 start depth and .075 flat depth on reversed male plug. It was very sloppy with way too much gap between the pocket and inlay piece. May have worked in VCP 8 but not in VCP 9. I no longer try to use this method.


I do not know your knowledge about CNC and Vcarve. As you have only 1 post on this forum, I think you are not a long time user of Vcarve. So, your post sounds strange: you're arguing that this method doesn't work properly while several experienced users explain it works perfectly. You can find numerous examples of fine Vcarve inlay work on this forum.

I do not see any reason it would work with V8 and not with V9 as there is no fundamental change in this area AFAIK.

If you identified a bug, please report it to Vectric. If not, post a file that didn't work, and you will get the required help.
Best regards

Didier

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 858
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: VCarve inlays and flat depth

Postby SCG » Sun Oct 21, 2018 9:44 pm

Yes, I am new to Vectric VCP and CNC for wood working. My reference to VCP 8 was based upon another thread shared by a long time user and seasoned v carve inlay VCP user. My results were identical to this users post, in that the gap between pocket and plug was always roughly 3/16th around entire inlay. This user also commented that the 3/16th gap was present even after tweaking the flat depth, start depth and flat depths of the file. After some serious thought, I did notice that any tools (V bits) available by choosing an engraving bit rather than V carve bit within V carve inlay tool path referenced the bit specs differently. V carve bits were saved under V bits using the diameter and the degree of v bit. In my case, I always use an Amana 1/4" shank with 60 degree v bit of .5 inch diameter. If I were to save this exact bit under my engraving bits, I would have been prompted to type in the bit's radius rather than diameter. And, I was also prompted to type in the tip measurement for v bit. I am aware V bits may have a tip measuring flat .001, .002, .003..or the true tip with 0.00 flat tip. Basically a true 0 tip like the Whiteside 1541 v bit which seems to be very popular for v carve inlays. I mention this because that would account for the consistent 3/16th gap on all my projects. I'm thinking by using a v bit saved as an engraving bit the radius measurement for engraving bit would all but eliminate that 3/16th gap present in every v carve inlay pocket/plug I've created and running repeatedly. Yes, I am new but do have a serious attention to detail as well as a highly driven research/study habit. This technique is the only method I've yet to pull off on the CNC/VCP. All other projects have run flawlessly.
SCG
 
Posts: 6
Joined: Thu Jul 26, 2018 8:02 am
Model of CNC Machine: Axiom AR8 Pro

Re: VCarve inlays and flat depth

Postby laflippin » Mon Oct 22, 2018 5:50 am

I'm not that experienced with Zank's V-inlay technique myself, having only been doing this since June of this year. However, I am not experiencing anything like what you have described...my male inlay pieces invariably "snap into place" in the female engraving, as Mike would put it.

Here are the parameters I generally use:

FEMALE ENGRAVING (w/ V-bit having 0.25" shank, 0.25" diameter, 60 degree angle)...the fIMAGE file
Start depth = 0.0"
Flat depth = 0.15" (i.e., 0.05" for the glue-gap)

MALE ENGRAVING (w/ same V-bit as above for the image, and an End Mill 0.25" for hogging out the bulk of the pocket around the image)

Setting up the two-step male engraving in my case uses off-sets around the image and a rectangle around the entire image + off-sets to define the pocket that will be hogged out. So, basically, I take the female image, create its mirror image, create an off-set 0.08" outward from the image, and then another offset 0.1" from the first off-set. Then, I create a rectangle around the whole shebang and save it as my mIMAGE file. For complex, multi-part patterns it is extremely useful to first "group" the original mirror image, then separately "group" the 0.08" off-set vectors, then separately "group" the 0.1" off-set vectors, after each off-set is created. It should be obvious why that's useful from the guidelines below:

Step 1 (V-bit 60): Open the mIMAGE file and (using the cursor and the SHIFT key) select two vectors for the V-carving step: The original male image and the 0.1" off-set vector. [Note: For complex, multi-part images they should be separately "grouped" so that the entire set of vectors in the original image are chosen with one click, and the entire set of 0.1" off-set vectors are chosen with one-click...while holding down the SHIFT key.)]
Start depth = 0.1"
Flat depth = 0.1"

Step 2 (EM.25): Open the mIMAGE file and select two different vectors for a pocket cut: The rectangle and the 0.08" off-set vector.
Start depth = 0.1"
Flat depth = 0.1"

This basic set of parameters is very reliable in my brief experience...I have been able to make several dozen inlay projects without any male-female compatibility problems with them.
Attachments
Inlaid dust collectors.JPG
laflippin
 
Posts: 46
Joined: Tue Jun 12, 2018 3:07 pm
Location: Cambria, CA
Model of CNC Machine: Piranha FX, Axiom AR 8 Pro+

Re: VCarve inlays and flat depth

Postby adze_cnc » Mon Oct 22, 2018 5:31 pm

SCG wrote:My results were identical to this users post, in that the gap between pocket and plug was always roughly 3/16th around entire inlay. ... This technique is the only method I've yet to pull off on the CNC/VCP. All other projects have run flawlessly.


Do you have an example file that doesn't work that you could post here? The only v-inlay projects I've done (admittedly few) have all worked flawlessly following the posted instructions.

I'm curious to know why it doesn't seem to work for you.

print.jpg
As FixitMike says it just locks into place.
User avatar
adze_cnc
Vectric Apprentice
 
Posts: 521
Joined: Sat Jul 27, 2013 10:08 pm
Location: Vancouver, BC, Canada
Model of CNC Machine: AXYZ 4008

Re: VCarve inlays and flat depth

Postby SCG » Sun Oct 28, 2018 5:53 pm

Yes, I can post a file. Should I upload my entire VCP pocket/inlay file. Or, just upload images of my mail/female pieces after running the file?
SCG
 
Posts: 6
Joined: Thu Jul 26, 2018 8:02 am
Model of CNC Machine: Axiom AR8 Pro

PreviousNext

Return to VCarve - General

Who is online

Users browsing this forum: No registered users and 20 guests