Best Bit for inlay

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro
Post Reply
jeffhcarter
Posts: 19
Joined: Tue Jun 12, 2018 8:22 pm
Model of CNC Machine: Shark HD4

Best Bit for inlay

Post by jeffhcarter »

Hello Everyone,
What is the best bit for doing an inlay word. I am using vcarve and a 30 Deg insert knife blade. The inlay does not fit snug into the pocket and does not drop in very deep. I did a 0 start point and a .2 flat bottom for the pocket. Then the same blade with a .1 start depth and a .2 flat bottom for the inlay. What am i doing wrong? Any help would be appreciated.
Thanks

User avatar
adze_cnc
Vectric Wizard
Posts: 4610
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Best Bit for inlay

Post by adze_cnc »

 
I've had this post on the to-answer list for a while now. Perhaps you've already solved the problem.
jeffhcarter wrote:
Sun Mar 24, 2024 12:56 am
What is the best bit for doing an inlay word.
I am fond of saying that there are no best practices only alternatives (it irritates the business-speak people...)

Here's an example of really small and finely detailed text using a 60-deg included angle bit (cutting edge to cutting edge) of Russell C.'s logotype.

Bit Angles
jeffhcarter wrote:
Sun Mar 24, 2024 12:56 am
I am using vcarve and a 30 Deg insert knife blade. The inlay does not fit snug into the pocket and does not drop in very deep.
Does that bit look like this 30 Degree Reversible Insert Solid Carbide Knife?

If so here's a case of the disconnect between manufacturer's incomplete labelling and Vectric product's expectations for the entering of bits.

If I were to enter that bit in the tool database it would be as a v-bit with a 60 degree included angle (as it is an equilateral triange). I believe the 30 degrees mentioned in the description really refers to the angle the cutting edges are ground to.

If you were to enter it as a 30 degree v-bit and calculated the toolpaths using that value but then tried cutting the parts with this 60 degree v-bit you'd quite probably encounter fit problems.

Inlay Start and Cut Depths
jeffhcarter wrote:
Sun Mar 24, 2024 12:56 am
I did a 0 start point and a .2 flat bottom for the pocket. Then the same blade with a .1 start depth and a .2 flat bottom for the inlay.
I can see from this that you are using the "default" values from the PDF located at "A Simple Way to Make Inlays". Be aware that the PDF really is a draft of the initial idea for tapered inlays. It is: 18 years old; doesn't consider further experiments with depths.

You might get a better understanding of the numbers by reading this post.

In short the start depth for the plug is the maximum amount of material (about 2.5mm) you expect to fit into the socket. As the socket's depth is about 5mm that means that there will be an equal amount of empty spaced below the inlay as the inlay thickness is.

If you are going to use 0.2" as socket depth you could easily use 0.17" for inlay plug start depth and 0.03" for the cut depth.

Are you using VCarve v12? If so there is a V-Carve Inlay toolpath that takes the place of creating two V-Carve / Engraving toolpaths.

If your VCarve version is less than 12 and it is VCarve Pro then this gadget might be of interest (especially with a Shark). If you are using Desktop and below v12 then this is a manual way to accomplish what the gadget can do.

Post Reply