Other Ginkgo Leaves

[SignTorch]

I finally got a look at the feather inlay video and that is INSANE - the finished inlay does not look like the drawing - because you cannot do a precise inlay with that method - the result is not predictable due thin details being lost for being less tall than the glue gap - and not tall enough to be visible in the cutting

I can't exactly match the drawing to the camera perspective but you can clearly see that the cut does not match the drawing

 

[blackmirror81]

Well I just walked in from the shop. I cut it in a piece of cedar, best thing I could find at the moment. It’s glueing up now and if the cold doesn’t bother it, I’ll surface it down tomorrow and see what we have! It slide right in, but my concern is the male piece is to thin for the female. We’ll find out soon. I used a V carve tooling path because it was the only way I could select a clearing tool. When I choose profile there wasn’t an option for clearing and when I chose pocket it didn’t see the vectors correctly and wanted to cut everything. Might be my problem there. Also didn’t see a way to chance offset.

 

[SignTorch]

that's amazing - you take straight pictures - you are a top .0000001 percenter

I'd use some fast drying glue for testing - ain't nobody got time for all that waiting to see what happens - lol - at least I am not that patient this close to Christmas - I just don't like uncertainty so I'd be injecting hot super glue from the back side to save 5 seconds at this stage

can't wait to see the result - afaik it should fit if both parts use the same depth settings - at least for this design with 15 deg bit - I don't think that's universally true with v-carve toolpaths - this design just happens to have a uniform minimum gap and component width for that one certain bit and cut depth(s) - so I don't see how it could go wrong

v-carve does not have pocket clearance - but I got to looking and at 9" tall I designed it to where a 15 deg bit .15 deep barely fits without .001 clearance or even .0005" to spare - so for a pocket toolpath that would've only worked if you scaled it 111% (about the same as 10" tall on large pattern) - in the image red is the male toolpath with .001 clearance and blue is the female - the one on the right is scaled 111% - the one on the left is original size where some of the cuts don't quite fit all the way - and that's where a v-carve toolpath would work but a pocket would not - I just have to make a drawing to wrap my brain around how v-carve works out - its not quite the same as pocketing - if you must add clearance when v-carving you can offset the drawing .001 - but that's splitting hairs so probably not that important

 

[SignTorch]

In my video I had to ungroup the design on the male side for the pocket toolpath to work right - apparently a group inside a container will not pocket correctly - not sure if that is why pocket wasn't working for you or not

 

[SignTorch]

and one thing I see that I don't like about my layout is it ends up with a .05" thick inlay with a .05" gap underneath - if the glue does not bridge that gap then that might be a weak link that requires different glue or a different strategy

 

[blackmirror81]

Great explanation. And yea I bet the grouping is what was causing the issue for pocketing. I did not think to ungroup them before making the tool paths

 

[blackmirror81]

Is there a way to decrease the .05 gap of the inlay? I’ll be surprised if the there isn’t a gap as the male piece was very thing, I’m sure it’s tapered slightly so we will see soon.

 

[SignTorch]

Is there a way to decrease the .05 gap of the inlay?

yes - the easiest way is to make the male go deeper and not change anything else

to make the gap below bottom of male .02" instead of .05" just add .03" (red) to the male start depth which becomes .08" (blue)

that makes male total depth of cut .18" and maintains .05" gap above top of female

optionally you could also decrease male cut depth (purple) to decrease the male total depth of cut and the gap above top of female by subtracting up to .03" from male cut depth (purple)

 

[blackmirror81]

Just finished planing this down, I used the CNC and I think I got some tear got from it. It came out great except the few spots. I’m guessing a slower feed and step would help a lot here. I’ll make those adjustments on my next few practices and I’ll be using walnut and maple. When looking close you can see the glue line around the edges. I bet those adjustments bring it in tighter!

 

[SignTorch]

that's more glue line than I expected

did you clamp it together good?

does your bit have a flat on it? if so then enter it as an engraving tool and set the flat width, and side angle is half the included angle (7.5)

or if part of the tip broke off then that's same as a flat - I don't know how they'd make a 15 deg v-bit without a flat without the tip breaking off

 

[blackmirror81]

I had it clamped pretty dang good, used a vise along with F clamps. The tip is to a point I believe. I feel like the depth changes we made to .08 is gonna make it perfect. When I glued up the maple and walnut the pieces were actually snug and I tapped it down then clamped the he’ll out of it. The cedar above the pieces weren’t sloppy but they fell right into each other.

 

[blackmirror81]

I’ve also been running carve first then clearing and I’m gonna try one that’s clearing then carve to see if there is any difference.

 

[blackmirror81]

Is there a place where I can learn more about calculation diameter of bits, angles, start and flat depth?

 

[SignTorch]

alright - sounds good - I wouldn't expect cedar to cut that much differently - it might help to decrease the bit pass depth to do multiple passes

and I'm assuming v-carve toolpath works here - but it does cut shallower to get through narrows and it does not cut shallower on the mating part so there is a fine line between how much shallower it cuts and how much gap there is before something bottoms out

I think we are ok using v-carve and increasing female total depth of cut to .18 because v-carve should not retract any more than we increased the total depth of cut which is .03 and the top gap is .05 so I think it should not bottom out - theoretically

but I'm only confident about my pocket toolpath calculations where the design is specifically sized for 15 deg v-bit, no flat, .15 max total depth of cut, pocket cut - and changing bottom gap to .02 means changing start depth to .08 and cut depth to .07 to not exceed .15 total depth of cut - and there is < .001 room to spare on width of cut in some places

it does help a lot to scale the design 111% to have > .001 room to spare - especially for v-carving to decrease v-carve retraction if tdoc is .18

my concern is if the bit were to have a flat or small break then that throws everything off a lot, enough to cause a major mismatch between male and female, enough to require recalculating all pocket toolpath depth parameters

I'd inspect the bit with a jeweler's loupe and check the specs because I find it hard to believe it doesn't have a flat or else the tip will break off

diameter calculations are simple geometry - but the difference between pocket and v-carve, straight and angled bits, clearance and start depth, and how that affects where the toolpath (bit centerline) is relative to the cut path (edge of part) at what depth is convoluted - I don't know of a learning resource to recommend offhand - I like to draw a diagram of the bit to see precisely what depth equals what width - in the diagram below that is a .125 x .15 rectangle and 15 deg bit cutting .03949 diameter at top of rectangle (.15 deep) - and I drew a .005 flat to show how much impact that would have, it would be cutting .04449 diameter at .15 deep and that would not work for this design even at 111% but maybe with v-carving it might work a little better - that's more complex to calculate what happens if the bit and toolpath type is not the same as originally specified

 

[blackmirror81]

Thanks for the explanation. What from that picture is making you think there is a flat spot or snapped tip? I thought it looked pretty good.

 

[SignTorch]

What from that picture is making you think there is a flat spot or snapped tip?

I'm not sure which picture you are referring to - my diagram is a reference to bits with .005" flat - in your pictures the inlay fit does not appear to be very tight

If I google "15 degree vbit" 4 of the first 5 results have .005" flat tips

the only one that does not have a flat is the $80 one with $30 blade inserts which is a 35 degree vbit

I cannot seem to find a 15 degree bit with any less than .005" flat

I think .005" flat is the standard minimum flat

I think a 15 degree bit with a sharp tip would literally break off from looking at it

I think I was absent minded to calculate the design as if there was such a thing but I'm not used to having this problem where .005" makes so much difference

 

[blackmirror81]

This is the bit I am using.

 

[SignTorch]

This is the bit I am using.

ahhh - .016" flat (fishtail) - I will have to recalculate - in your tool database you set the bit to an engraving tool and then it will let you enter the flat diameter - and you enter the side angle (7.5) - give me a few and I will refigure the measurements

 

[blackmirror81]

Got all that setup for tool paths and it looks much cleaner. I ran pockets as suggested this time by in grouping. Is there any change to start and flat of the female piece or only male? I won’t be able to test till Monday. I also scaled to 111%

 

[SignTorch]

Is there any change to start and flat of the female piece or only male

I deleted my previous diagrams and response - it was half baked - this is better

15 degree engraving bit with .016" flat

For the female: start depth = .02" and cut depth = .08"

For the male: start depth = .06" and cut depth = .04"

MUST SCALE THE DESIGNS UP AT LEAST 111%

 

[SignTorch]

new layout

 

[SignTorch]

new video

 

[blackmirror81]

I finally got the parts back in to run my CNC. This newest version isn’t cutting well. The pieces are now very thing on the male piece. In our old thread where we were working through it, the last version I had cut and glued it it came out excellent. Do you have a copy of the post so I could see what has changed to make it no longer working for the inlay?

 

[SignTorch]

I finally got the parts back in to run my CNC. This newest version isn’t cutting well. The pieces are now very thing on the male piece. In our old thread where we were working through it, the last version I had cut and glued it it came out excellent. Do you have a copy of the post so I could see what has changed to make it no longer working for the inlay?

I undeleted all of the old posts.....

I got to looking and the reason why they use zero female start depth on the v-carve inlay technique is because they cut the female into a (nearly) finished part and they do not face any more material off of the female after the inlay is set, they just sand the inlay flat, whereas the way I described it allows for facing off the inlay and female part another .02" deep after the inlay is set, like a final finish pass on the entire part.

 

[blackmirror81]

Thank you for the quick response! The one that cut well was the one you had posted about on 12/14. The latest version the thing sections were much thinner and fragile. Most broke off during the cut. I have ordered 2 newer 15 degree bits to try, with a .005 tip. The previous ones kept snapping the tips off and wouldn’t make it through 2 cuts.