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 jtcdudeman » Sat Jul 14, 2012 3:57 am

I've gone through this thread and checked out the PDF file. I have an extremely silly question, but I haven't had much success playing with inlays in the last day or two that were slightly more complex than a star. This method will work in both Aspire and VCarve the same?

I have been trying to figure out why I cannot do the male inlay with a V-bit. I get locked out and not offered a V-bit as an option. What could I be doing wrong?
jtcdudeman
 
Posts: 11
Joined: Thu Dec 02, 2010 10:43 pm
Location: Sugar Hill, GA USA

Re: A simple way to make inlays

Postby tmerrill » Sat Jul 14, 2012 6:22 am

There are two different approaches to doing inlays and it appears you have them mixed up in your mind.

Aspire/VCP include an Inlay tool which is designed to use straight sided bits (end mills) to create the male and female parts (and will not accept a v-bit). What the tool does that is special is that it modifies both the male and female parts for the radius of the bit so the parts will fit together perfectly. This approach works well with large inlays or simple designs.

The other approach is called the V-carved inlay and was developed by a couple of users. This does NOT use the Auto Inlay tool, but the V-carved toolpath with a v-bit and is what the PDF document is about. It's advantage is toward small and detailed designs like the projects you have seen people post in this thread.

Best thing to do is learn about each technique and see which one is better suited for the job you want to do. There is a tutorial video here that will help introduce you to the Auto Inlay tool. Look at #9:

http://www.vectric.com/WebSite/Vectric/ ... _mach.html

Tim
tmerrill
Vectric Archimage
 
Posts: 4794
Joined: Thu May 18, 2006 3:24 pm
Location: North Carolina
Model of CNC Machine: ShopBot

Re: A simple way to make inlays

Postby 7.62x54r » Sun Jan 06, 2013 11:17 pm

I just stumbled across this and am excited about trying it out. I made one simple test of a 1.125" star out of walnut inlaid in baltic birch with a 90 degree bit. It has issues, probably from a clamp time of only 1 hour and possibly incorrect speeds, but I see potential. What I would like to do in this post is a recap of the setting values as I understand them, along with a couple I haven't seen mentioned, and get some feedback from the members who have more experience with this method of inlay. (I mostly cut 2D parts from 3/4" plywood with a straight bit but want to get into more interesting work.)

For my purposes I plan on using the V bit for flat clearance as I don't have an ATC and have always been concerned with knocking the CNC out of alignment when changing bits by hand in the middle of a job. I also plan on using TiteBond II for my gluing and only working in wood for now as that's what I do. Maybe I'll get into solid surface material and other glues later, but for now I want to stick pretty close to what I know already.

Bit zeroed on the top of the material for both cuts.
Pocket start depth: 0.0"
Pocket flat depth: 0.3"
Pocket stepover (clearance and final) 3%
Inlay start depth: 0.1"
Inlay flat depth: 0.2"
Pocket stepover (clearance and final) 15%
The above values result in a contact surface of 0.1" measured in the Z axis and a 0.1" clearance between the bottom of the inlay and the bottom of the pocket.

It is my understanding that a 60 degree bit gives better results than a 90 degree bit.

Now what I have not seen mentioned in this thread, the PDF, or the video is the rpm and the feed rate. I understand that those depend on the material, but as a relative newbie to anything but hacking away at plywood I could use some help. I expect to work primarily with maple and walnut (relatively cheap and great contrast) but also inlay the walnut into the baltic birch plywood I use.

What rpm should I be running my PC 7518 on my old (circa 2000) PRT ShopBot for woods like walnut and maple and what should the X/Y feed rate and Z plunge rate be for 1/2" 90 degree and 1/2" 60 degree bits.

Is there anything else I'm missing?

Thanks in advance.
7.62x54r
 
Posts: 27
Joined: Fri Nov 05, 2010 2:41 pm

Re: A simple way to make inlays

Postby Paul Z » Mon Jan 07, 2013 1:09 pm

I keep the rpms very high and cut speed down to 0.5"/sec. This is one time I don't mind creating dust instead of chips. I will often cut the pieces twice to get the best possible fit. Use your sharpest bits to minimize chipout.

Titebond II is a very good choice. Use a lot of it and let it set for a full day. Use lots of clamps. You are trying to force side contact to the point of deforming the wood to make a fit with no gaps.

I encourage you to post your results, even the failures. I learn more from the failures.

Paul Z
Paul Z
Vectric Wizard
 
Posts: 516
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Re: A simple way to make inlays

Postby 7.62x54r » Mon Jan 07, 2013 2:03 pm

Paul, thanks for the answer. I've ordered new Freud bits as the only V-grooves I had were second hand of unknown use and initial quality. When you say "cut the pieces twice" I'm guessing you just run the same file over again to clean up any "fuzzies", correct? You're not making a shallow pass and then a full depth pass.

So far all I have is one small test star. I wouldn't call it a success or a failure, just a poor example. I have several projects in mind and will post them when I get them done. This is strictly for "fun" and most of my shop time is spent on more mundane work to put beans on the table.

Thanks again.
7.62x54r
 
Posts: 27
Joined: Fri Nov 05, 2010 2:41 pm

Re: A simple way to make inlays

Postby RhoTu » Wed Feb 06, 2013 11:42 pm

I was wondering if any of the inlay gurus (ie. experienced) are successfully using male inlays that are less than 0.5 in? It seems like a lot of wastage of expensive material. A 0.1 in allowance for glue seems excessive. I will be trying my first attempts in the next couple of weeks but thought I would ask here before experimenting on my own. Thanks in advance for any responses.
RhoTu
Vectric Craftsman
 
Posts: 138
Joined: Mon Dec 29, 2008 10:12 pm

Re: A simple way to make inlays

Postby Hurricane » Thu Feb 07, 2013 5:16 am

I do inlays of .120 in flat and round objects. I use flat cut bits not the vgrove style as this subject. If you do these type you need to use tiny bits. I typically use .030 bits that have a depth of cut of .125... If you want more info you can email me and I will be glad to assist in any way I can...
Attachments
IMG_0706.JPG
IMG_0753.JPG
IMG_0756.JPG
"Whitey"
K2 Devices/4 axis
Corel Suite
Vcarve Pro6.5
PhotoCarve
Aspire4.5
User avatar
Hurricane
Vectric Apprentice
 
Posts: 96
Joined: Sat Aug 19, 2006 11:53 pm
Model of CNC Machine: K2 4 axis

Re: A simple way to make inlays

Postby rscrawford » Thu Feb 07, 2013 3:42 pm

RhoTu wrote:I was wondering if any of the inlay gurus (ie. experienced) are successfully using male inlays that are less than 0.5 in? It seems like a lot of wastage of expensive material. A 0.1 in allowance for glue seems excessive. I will be trying my first attempts in the next couple of weeks but thought I would ask here before experimenting on my own. Thanks in advance for any responses.


I cut almost all of my male inlays out of .1" thick material, and have usually only about .02" glue gap (or if the male comes to a point, I'll sand off the very tip of the point).

DSC_2412.jpg


Sorry this picture is so small. I tried to find the larger version, and I'll post it when I find it.
DSC_2413.jpg


closeup.JPG


This picture shows what the pieces look like when they are glued in (half done planing off the excess). I don't clamp my inlays, they just set in place with glue. Inlays really show the precision of your machine.
planing.JPG
Russell Crawford
http://www.cherryleaf-rustle.com
User avatar
rscrawford
Vectric Wizard
 
Posts: 938
Joined: Mon Jan 17, 2011 6:49 pm
Location: Wetaskiwin, Alberta
Model of CNC Machine: CAMaster Cobra 408 ATC with recoil

Re: A simple way to make inlays

Postby RhoTu » Thu Feb 07, 2013 4:41 pm

Would you be willing to outline your settings used for this approach?

60 or 90 degree bit?

It looks as if you are cutting all the way through your inlay material. What method are you using to hold the inlay material in place while cutting?
RhoTu
Vectric Craftsman
 
Posts: 138
Joined: Mon Dec 29, 2008 10:12 pm

Re: A simple way to make inlays

Postby rscrawford » Thu Feb 07, 2013 5:04 pm

I use a 60 degree v-bit and I cut almost all the way through my male inlay (I leave .005" onionskin, then flip the piece over and gently sand the back to release the male pieces - most of mine are very fragile).

I cut the male pieces with a prism toolpath, truncated .02" shallower than my v-carved female cut. Then I offset the vectors outwards by .08" and do a v-carve between the original vector and the offset. This gives me a little extra thickness to the male inlay, without touching the original prism cut.
Russell Crawford
http://www.cherryleaf-rustle.com
User avatar
rscrawford
Vectric Wizard
 
Posts: 938
Joined: Mon Jan 17, 2011 6:49 pm
Location: Wetaskiwin, Alberta
Model of CNC Machine: CAMaster Cobra 408 ATC with recoil

Re: A simple way to make inlays

Postby rscrawford » Thu Feb 07, 2013 10:26 pm

I forgot to add an important note! When I offset the vectors and do a v-carve between the vectors and the offset vectors, I START the v-carve at the depth I set the prism cut. This starts the v-carve at the bottom of the prism cut, essentially extending the depth just a little more, but leaving the bottom of the prism cut untouched(which is the edge that shows once it is glued in place).
Russell Crawford
http://www.cherryleaf-rustle.com
User avatar
rscrawford
Vectric Wizard
 
Posts: 938
Joined: Mon Jan 17, 2011 6:49 pm
Location: Wetaskiwin, Alberta
Model of CNC Machine: CAMaster Cobra 408 ATC with recoil

Re: A simple way to make inlays

Postby hmonnier » Tue Jul 16, 2013 3:00 pm

I have gone thru all 19 pages, and want to try this out. I read in one of the posts that the writeup was corrected, was that ever posted, or is the one there correct (even though it has a warning message). If there are changes, could someone let me know what they are?
Thank you,
Henri
Henri
Joe's 4x4 Hybrid (modded), Aspire
hmonnier
 
Posts: 2
Joined: Sun Mar 03, 2013 9:07 pm
Location: Murphy, NC
Model of CNC Machine: Joes 4 x 4 Hybrid (modded)

Re: A simple way to make inlays

Postby Paul Z » Tue Jul 16, 2013 5:57 pm

Look at the very bottom of the first post. There's a pdf file.

Paul Z
Paul Z
Vectric Wizard
 
Posts: 516
Joined: Sun Apr 30, 2006 10:04 pm
Location: New Hampshire, USA
Model of CNC Machine: shopbot PRT Alpha 96x48

Solid toolpath preview as relates to inlays

Postby llwood » Thu Jun 19, 2014 2:18 am

As part of trying to figure out inlays, I came across this comment from May, 2012.

This can be demonstrated by turning solid on in the preview tool path and then looking at the drawing.


I thought it would be a great idea to turn on solid when previewing the toolpaths and then seeing the area carved out by the cutting tool, but it doesn't seem to work. I created the attached test file to demonstrate this.

To see what I mean, open the attachment and go to "Preview Toolpaths." At the bottom, make sure both "Show 2D previews" and "Solid" are checked on. Then preview the toolpaths. Notice that the bottom two boxes are of different sizes in the 3D preview. I put in some vertical lines to make this obvious. Now, make sure there is a checkmark next to each toolpath on the toolpath list, and then click on the tab to go back to the drawing view. In this file, the tab will be labeled "Test of solid toolpath previews.crv" Notice the solid colored outline is the same for each of the bottom 2 squares, relative to the square. If you switch back and forth between the 3D view and the drawing view, you see that the squares are carved differently on the 3D view but they show up the same on the drawing view. Do you see what I mean?

It seems to me that the "solid" toolpath preview in the drawing tab should be shaded anywhere the tool cuts at z=0. This isn't the case, because the tool is cutting places that aren't shaded. So do I misunderstand this feature, or does this indicate a bug in the software? I'd appreciate any help in understanding this feature.

Thanks,
--Andy
Attachments
Test of solid toolpath previews.crv
(85.5 KiB) Downloaded 213 times
User avatar
llwood
Vectric Wizard
 
Posts: 382
Joined: Sun Nov 18, 2012 5:07 pm
Location: Dillsburg, PA
Model of CNC Machine: Legacy Maverick

Re: A simple way to make inlays

Postby BrianM » Thu Jun 19, 2014 9:17 am

Hi Andy,

Then preview the toolpaths. Notice that the bottom two boxes are of different sizes in the 3D preview


This is because you have told the software that the second toolpath starts at Z -0.19 so the 2d preview shows what the toolpath would machine assuming that the material is starting at Z -0.19.

This is the intended behavior as many jobs involve pocketing out an area and then machining in the base of the pocketed area. If you imagine v-carving text in the base of a pocket, showing the outline of the v-carving at the surface level would be completely useless.


Brian
Brian Moran
Managing Director
Vectric Ltd.
User avatar
BrianM
Vectric Staff
 
Posts: 1965
Joined: Mon May 16, 2005 10:15 am
Location: Redditch U.K

PreviousNext

Return to VCarve - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 5 guests