blackmirror81
member
Hi this is the guy from Facebook. I'm wanting to make this an inlay out of walnut and maple. I believe I posted a photo on FB showing the cutting board a guy did. I will be making this inlay for two side tables. I'm still pretty new to CNC and what bits do what. I'm using Aspire and running a Onefinity. I noticed a few of the petals weren't quite symmetrical if that is the right word. You had also brought up some points about the sizing. I am very excited and very happy you were so willing to help me conquer this. Thank you
SignTorch
Artist
hey, welcome aboard, my apologies for the delay, electricity went out this morning for most of the day, in the middle of a drawing, I hate when that happens....
It helps to know about what size do you want the drawing to be for your project.
And do you want the petals or certain petals to be more symmetrical? If so it helps to be more specific like "can you make the 3rd leaf up from the bottom a little more symmetrical?". I'm a hypochondriac when it comes to uncertainty. But only when it comes up. I usually don't get and don't need much more than an image and maybe one number for a size, but I'm new to inlays and so the devil is in the details on this project.
It helps to know about what size do you want the drawing to be for your project.
And do you want the petals or certain petals to be more symmetrical? If so it helps to be more specific like "can you make the 3rd leaf up from the bottom a little more symmetrical?". I'm a hypochondriac when it comes to uncertainty. But only when it comes up. I usually don't get and don't need much more than an image and maybe one number for a size, but I'm new to inlays and so the devil is in the details on this project.
blackmirror81
member
When I imported the picture into Vectric, the two leaves I marked came out strange when traced. I would like the design to be 10"-8" by whatever the needed width is to maintain the appearance it is now. I"m brand new to CNC in general and taking this on for a Christmas project for my mom. She got some bad medical news this summer and I really need to make this Christmas count. She fell in love with this design and I will be replacing to side tables with this in Walnut and maple.
This is the video that everyone touts as the go-to instruction for inlays.
And here is the video of this carving being cut.
This is the video that everyone touts as the go-to instruction for inlays.
blackmirror81
member
I believe the guy in the video making the inlay board used a 30 degree V bit and it came out. Could we make the width adjustments for the lines work for a 30 degree?
blackmirror81
member
I'm guessing a 30 degree and a 1/8 endmill would work? I'm still learning but I'm very anxious about this process. I know getting the toolpaths is 99%
SignTorch
Artist
Trace? - you import the SVG, scale it to size as desired, and then edit/curve-fit-vectors, and you do not edit/trace-bitmap
I will modify the leaf - that does look a little strange...
SignTorch
Artist
He tried a 30 deg v-bit and a 15, and he chose the 15 because the 30 did not leave enough height to work with on the thin parts and he definitely used a 15 deg v-bit on the dark wood. I don't think its feasible to use a 30 v-bit on that design at that size because the lines and gaps are really narrow and you'd have the same problem he did, not much height, and the problem with that is there's very little engagement between the two parts and very little margin for error in cut depth when you face off the inlay, a little difference in height makes a lot of difference in the shape of the inlay, whereas a 15 v-bit gives more engagement and more margin for some error.
All I can do is balance the width of the parts and the gaps to be more equal so that one is not much narrower than the other, because the narrowest space is what determines how much height and engagement you will have to work with. Then you can use a 15 or 30 v-bit, but 30 is less user friendly, and the design would have to be modified a lot to be ideal for 30, and 30 is not ideal for this type of design.
SignTorch
Artist
Well count me in and I will get this ready for you asap because you will have to practice and test these procedure(s).
Mom's are so special, and bad news is so difficult, I know all about that, if you scroll way down on my facebook page - https://facebook.com/gary.dewitt.73 - every second counts - so I do wish you and her the very best
blackmirror81
member
I liked seeing the pictures of you climbing with her there. Something I would do. I tried my hand a climbing a few years ago, never got the hang of it but I stop and watch the guys when I see them working. It’s part circus act part art. I really appreciate the break down of his video. I ordered some 15 degree bits! Do you think a 1/8th inch up cut for clearing?
SignTorch
Artist
SignTorch
Artist
This shows a .04" wide inlay section - with .05" assembly clearance - .1" engagement - 15 deg. bit
I don't know about the inlay tool path or if it is for tapered inlays or not - this is the same as and I would use standard pocket operations
Pocket outside the inlay and pocket inside the bed, both with .05" starting depth, and .1" cutting depth - final face off removes .05" of bed
The red line is the final plane where the cut is to be the same shape as the design - hence the .05 start depth
I don't know about the inlay tool path or if it is for tapered inlays or not - this is the same as and I would use standard pocket operations
Pocket outside the inlay and pocket inside the bed, both with .05" starting depth, and .1" cutting depth - final face off removes .05" of bed
The red line is the final plane where the cut is to be the same shape as the design - hence the .05 start depth
blackmirror81
member
Thank you for the work put into explaining that post, but I'm still confused. Garrett Fromme's video says to use:
→ For the Female inlay component
Start depth 0.0
Flat depth 0.11 (2.794mm)
→ For the Male Inlay component
Start depth 0.09 (2.286mm)
Flat depth 0.02 (0.508mm)
But he is using a 90 degree v bit on a totally different file, a feather. When I try to use his value or when I try to use yours, the preview in Aspire show material not removed. I used the SVG like you told me. Would you mind explaining it once more like you are talking to a 5 year old. I don't really grasp the diagram above.
→ For the Female inlay component
Start depth 0.0
Flat depth 0.11 (2.794mm)
→ For the Male Inlay component
Start depth 0.09 (2.286mm)
Flat depth 0.02 (0.508mm)
But he is using a 90 degree v bit on a totally different file, a feather. When I try to use his value or when I try to use yours, the preview in Aspire show material not removed. I used the SVG like you told me. Would you mind explaining it once more like you are talking to a 5 year old. I don't really grasp the diagram above.
blackmirror81
member
Sir, I don't know your actual name, I'm Mike. But every once in awhile I'm blown away by the genorisity of the internet and its ability to reach people. I was just telling my wife about the effort you put into making a video to help me and make me successful. Thank you very much for your time and effort. I followed your instructions and I believe I have what should be working toolpaths now. I am waiting for my bits to come in tomorrow and I will be able to try this out on some sample pieces. I will report back. My version of Aspire is 11.0 and when you made the pocket toolpath it does not give me an option for using a clearance tool, but I can add multiple bits into it and change the order. The program seems to know to use them as a clearance ( endmill, then v bit ) I'm hoping that is right. When doing the female piece, is there a difference between running it as a v carve vs pocket?
SignTorch
Artist
yes version 11 has multi-bit clearance tools so you could also run a .06 or .09 flat endmill to save time and wear on the v-bit cleaning out where .125 won't fit - that's not too important for an inlay because you don't see or finish the bottom of the pocket - but for regular pocketing there is a huge benefit to not having to use the v-bit for clearance any more than necessary.
I would not use a v-carve toolpath for an inlay because the purpose of v-carving is to retract the depth as necessary to cut sharp corners even to zero depth at the tip of a sharp point. I'd only use v-carve toolpath for v-carving.
Which raises a question that I need to check the design on. If there is a corner sharper than the radius of the 15 v-bit at .1 or .15 deep then the male and female will not cut exactly the same at that corner. And that would be where the inlay toolpath comes in to play because it takes care of that issue. But I am not at all familiar with the inlay toolpath.
I will check the design and let you know if there is a problem or not. I did round everything off but I did not consider the exact minimum radius required.
With a properly rounded off design then pocket, v-carve and inlay toolpaths would all do essentially the same thing, with the same tool, but they would behave differently on sharp corners if the design was not properly rounded of for the tool, from what I gather, This is why I like to help people, I love this stuff. Like, I knew it was good practice to round off my designs but this is one of the few cases where it is very important and not optional and not simply good practice. So I'm interested to see if I accidently got it right or if it is still not correct.
I would not use a v-carve toolpath for an inlay because the purpose of v-carving is to retract the depth as necessary to cut sharp corners even to zero depth at the tip of a sharp point. I'd only use v-carve toolpath for v-carving.
Which raises a question that I need to check the design on. If there is a corner sharper than the radius of the 15 v-bit at .1 or .15 deep then the male and female will not cut exactly the same at that corner. And that would be where the inlay toolpath comes in to play because it takes care of that issue. But I am not at all familiar with the inlay toolpath.
I will check the design and let you know if there is a problem or not. I did round everything off but I did not consider the exact minimum radius required.
With a properly rounded off design then pocket, v-carve and inlay toolpaths would all do essentially the same thing, with the same tool, but they would behave differently on sharp corners if the design was not properly rounded of for the tool, from what I gather, This is why I like to help people, I love this stuff. Like, I knew it was good practice to round off my designs but this is one of the few cases where it is very important and not optional and not simply good practice. So I'm interested to see if I accidently got it right or if it is still not correct.
SignTorch
Artist
There was a spot where I had not rounded the corner (red) and that would have left a gap between the male and female. And I think that the inlay toolpath would have compensated for that (theoretically). It also helps prevent the wood from chipping off on that sharp point.
And actually, that might be sharp on the male and round on the female so that instead of a gap it would be an overlap and they would not fit together at all.
Definitely must do a test/practice cut to make sure. And it won't hurt to scale the design from 9" to 10" tall because that is the bare minimum radius for that tool at that depth.
And actually, that might be sharp on the male and round on the female so that instead of a gap it would be an overlap and they would not fit together at all.
Definitely must do a test/practice cut to make sure. And it won't hurt to scale the design from 9" to 10" tall because that is the bare minimum radius for that tool at that depth.
SignTorch
Artist
The only other issue I can think of is if you might should add .001" pocket allowance on both male and female pockets for glue and for clearance in general. You would never cut two non-tapered parts exactly the same size if they are supposed to fit together, although the inlay is tapered so the two parts will settle together, but adding .001" pocket allowance would eliminate the inevitable interference between two parts that are exactly the same size for a more perfect fit (with room for glue).
And the v-carve toolpath doesn't have pocket allowance, so that's another difference between v-carves and pockets.
And the v-carve toolpath doesn't have pocket allowance, so that's another difference between v-carves and pockets.
SignTorch
Artist
I edited the post that is right before the new files. I added a paragraph about scaling. I'm now all worried about the potential for some slight interference that would prevent a perfect fit. But I do believe that between the taper and the flexibility of the wood and some clamping pressure it will work without being perfect. But on a 7.5 deg taper a .001" misfit cause a .008" height shift.
So, scaling the design from 9" to 10" tall and add .001" pocket allowance on male and female sounds like a good idea to me.
But like I said, I'm a hypochondriac about uncertainty, once I get to thinking about it.
So, scaling the design from 9" to 10" tall and add .001" pocket allowance on male and female sounds like a good idea to me.
But like I said, I'm a hypochondriac about uncertainty, once I get to thinking about it.
blackmirror81
member
I bought some wood today and my bits should be there tomorrow to run some test pieces. I will report back soon with my outcome. When you say inlay tool path, you are referring to the inlay tool path option that makes you select make or female right?
SignTorch
Artist
yes - unless I misspoke - where I call the male part of this project the inlay where that toolpath is a pocket
but generally when I say inlay toolpath it would mean the special toolpath for male and female components
which appears to be for cutting the male part out, with an optional step, and I just don't see that it allows for pocketing out around the outside of the male part for this type of inlay, unless I'm wrong or V11 has features that I don't know about.
I am just vaguely aware that it does tool size corner compensation and that is important on this and that type of inlay, and I can't believe I didn't think to check that on this design until you asked about v-carving