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
autogateman
Posts: 12
Joined: Fri Mar 02, 2012 2:44 am
Model of CNC Machine: sx3

Re: A simple way to make inlays

Post by autogateman »

ok guys, I have read and re read this thread, and can not figure out why the inlay start depth is not 0. why couldnt you have a 0 start depth, and just profile with the v bit down to a level slightly deeper than the depth of the pocket??

User avatar
zeeway
Vectric Wizard
Posts: 3157
Joined: Thu Feb 11, 2010 9:24 pm
Model of CNC Machine: Self-built
Location: SC, USA

Re: A simple way to make inlays

Post by zeeway »

My understanding:

In order to fit, the shapes on the male inlay and the female pocket have to be the same at some specific plane (layer) in the combined workpiece. If you cut the exact shape on the surface of the male inlay piece, you need the mating "exact" shape to be below the surface of the female piece so your inlay will have more than zero thickness. Hope this makes sense.

Angie

dturk
Vectric Apprentice
Posts: 20
Joined: Mon Dec 27, 2010 2:22 pm
Model of CNC Machine: Legacy Arty58 / Shark Pro
Location: Land O Lakes, Fl

Re: A simple way to make inlays

Post by dturk »

This is my first post and I have been trying to do the Vinlays for the past three weeks. It seems everyone is success full, but I'm missing the boat some how.

When I create the male inlays they are always bigger than the Female pockets

Female Pocket:

When I use the following instructions:

3. Open the ToolPaths Tab on the right side of the interface
4. Select the "Create V Carve / engraving toolpath" icon.


I get a V-cut on the inside of the line. (This can be demostrated by turning solid on in the preview tool path and then looking at the drawing)

Male Inlay:

In the pdf the instructions are the same, except a box was created around the object.

6. Open the ToolPaths Tab on the right side of the interface
7. Select the "Create V Carve / engraving toolpath" icon.


When this is calculated this creates a V cut outside the object. There fore the two objects can't mate. I can solve this by using a Profile cut and selecting Inside line cut path. But this does not seem right. I have been searching for a tunnable or configration parmeter in both Vcarve Pro and Aspire, but I have not found any todate.

Can anyone help. Thanks
Attachments
Problem.jpg

User avatar
Adrian
Vectric Archimage
Posts: 10873
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: A simple way to make inlays

Post by Adrian »

I presume you are setting the start depth for the male part correctly?

Have you cut the parts or are you looking at the previews and thinking they won't fit? The pictures you attached look ok to me.

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

Both parts must be v carved for this to work. They look like they won't fit but they do (at least so far). It can be difficult to get the parts to fit because there is no indication that you are close until they suddenly fit. I always fit mine dry (no glue) and make pencil guide marks. That allows me to quickly find the fit point when I have the parts wet with glue.

If done correctly, the male and female parts will contact each other only on the v carved sides. Heavy clamping pressure wedges the two parts together. (One user reports that he uses a hammer! :shock: )

Using lots of glue helps to fill the void in the bottom of the female part. Give the glue plenty of time to set before cutting the backing off the male part. If you use conventional wood glue, wait at least 24 hours. The waiting is the most difficult part of this process!

It seems as though a 60 degree v bit is being used more often than a 90 degree bit.

Paul Z

dturk
Vectric Apprentice
Posts: 20
Joined: Mon Dec 27, 2010 2:22 pm
Model of CNC Machine: Legacy Arty58 / Shark Pro
Location: Land O Lakes, Fl

Re: A simple way to make inlays

Post by dturk »

Thanks. I have enclosed a simple crv drawing maybe this well help. The Maple leave was one that I pulled off a earlier post to see if I was doing something strange.

I have also enclosed a drawing to help explain the information. When I V carve the inlay the distance for line A is the same distance for line B in the pocket. For it fit I would think it should I would think that line A should have the same length as line C in the pocket so the two could mate.

The carve file have included, is the one I have been playing with and I think I have carved out 22 times trying understand (Hard Headed) On this file I made both the inlay and the pocket size the same hieght -- So they should mate .

Thanks again for your help.
Attachments
problem2.jpg
inlay Test.crv3d
(620.5 KiB) Downloaded 261 times

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

A should be slightly larger than C. The male part does not go all of the way to the bottom of the female part.

The file you attached is not the maple leaf.

Paul Z

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

You do not need to resize the artwork. It just needs to be flipped left to right. If you do resize either one, the inlay will not work.

Paul Z

dturk
Vectric Apprentice
Posts: 20
Joined: Mon Dec 27, 2010 2:22 pm
Model of CNC Machine: Legacy Arty58 / Shark Pro
Location: Land O Lakes, Fl

Re: A simple way to make inlays

Post by dturk »

Paul Z, Thank you for your help. I really do enjoy your aritcles and posts. This weekend I will make the maple leaf. It is the one that was posted earlier. It seems to be the one everyone has used for thier first inlay. Based on what I have done so far, I don't see how it is going to work. I have been using mostly hardwoods so they don't compress very well.

I'm also building a hydrolic press with two bottle Jack's. If 12 tons of preasure can't mate the the two halves I don't know what will.

Thanks again for your help.

Daryl
Attachments
Maple leaf.crv3d
(485 KiB) Downloaded 307 times

User avatar
Adrian
Vectric Archimage
Posts: 10873
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: A simple way to make inlays

Post by Adrian »

You've got the settings for the male and female parts the wrong way around.

The start depth goes onto the male part (the one surrounded by the rectangle) at 0.1" with a cut depth of 0.2" if you're following the instructions exactly.

For the female part the start depth should be 0.3" with a start depth of 0".

You're also using different v-bits for each toolpath. You must use the same v-bit for each toolpath or it won't work.

dturk
Vectric Apprentice
Posts: 20
Joined: Mon Dec 27, 2010 2:22 pm
Model of CNC Machine: Legacy Arty58 / Shark Pro
Location: Land O Lakes, Fl

Re: A simple way to make inlays

Post by dturk »

Thank you Adrian. This whole thing has been driving me crazy. It is so logical it should work. The instructions are clear, but it just doesn't seem to work correct. I have recalibrated my system, and re-installed the software, and purchased bits, and I ran Paul Z's angle validation process. thinking I have been doing something strange.

Daryl

tmerrill
Vectric Archimage
Posts: 4797
Joined: Thu May 18, 2006 3:24 pm
Model of CNC Machine: ShopBot
Location: North Carolina

Re: A simple way to make inlays

Post by tmerrill »

Daryl,

Inlays are one of the quickest ways to determine if your machine is properly adjusted and cutting accurately. Not saying that is an issue here, but may be part of it. We know the process works, just look through the thread at what people have produced.

I would suggest you forget the leaf and pick a simpler design, such as a star, to practice and troubleshoot with. Once you get that working, then any design should work for you.

Tim

Paul Z
Vectric Wizard
Posts: 517
Joined: Sun Apr 30, 2006 10:04 pm
Model of CNC Machine: shopbot PRT Alpha 96x48
Location: New Hampshire, USA
Contact:

Re: A simple way to make inlays

Post by Paul Z »

Has anyone used the V inlay process on text without first changing the text to vectors? If you used text directly, how did it turn out?

Paul Z

User avatar
rscrawford
Vectric Wizard
Posts: 985
Joined: Mon Jan 17, 2011 6:49 pm
Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408
Location: Wetaskiwin, Alberta
Contact:

Re: A simple way to make inlays

Post by rscrawford »

I do inlays using text all the time. I vcarve the text, then prism carve the male inlay. To make things easier, I'll sometimes offset the text, and then do a v-carve between the offset and the text, starting the v-carve at the depth of my prism base. This simply extends the prism down further so I don't have to clean up the area between prisms on the inlay. Sometimes I'll just offset the text and then prism cut the offset, but sometimes with fine text this will lose some of the detail.
Russell Crawford
http://www.cherryleaf-rustle.com

mountaincraft
Vectric Craftsman
Posts: 229
Joined: Sat Apr 30, 2011 2:30 pm
Model of CNC Machine: DIY 4' x 8' CNC Router/Plasma
Location: Shingletown, Ca. 96088

Re: A simple way to make inlays

Post by mountaincraft »

This is awesome! Just what I was looking for.. Thanks!

Post Reply