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: 2
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: 8434
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: 472
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: 2
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 Craftsman
 
Posts: 249
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: 11
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: 1421
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (modified)

Previous

Return to VCarve - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 7 guests