How to Create Perfect V-Carve Inlays on your CNC

hey folks Winston for carbide 3D here we're always on the lookout for ways to improve our products and add value for our users and one area that's been on our radar is the vcarve inlay functionality in carbide create inlay mode is included in the basic version of carbide create version 7 which is free for all owners of carbide 3D cnc's but in its prior iteration there were certain cases where our workflow could produce an imperfect inlay and that really bugged us so we took a step back did a lot of testing worked through some issues we found and are back with what is effectively inlay mode 2.0 for carbide create this new workflow is simpler than its predecessor while consistently yielding better results across the board today I'm going to show you how to use this updated vcarve inlay mode with an example in the form of a drink coaster the materials I'm going to use are bamboo plywood and some Walnut we'd recommend using fine grained hardwoods for inlays like Maple or walnut since you'll need your inlays to hold fine details without chipping out when machined softer Woods like Pine and coarser grained Woods like red oak may not retain delicate features as well the bare minimum of tools I'll need for this project are an e in endmill like the carbide 3D 102 and a 60° vbit in this case are 302 if you're working with materials that tend to have fuzzier edges when cut using down cutting endmills like the Amanda 462000 DK or carbide 3D 251 may help but we can talk about that more when we're Machining let's jump into the latest version of carbide create and get started with a design we're going to need to draw up two parts for this inlaid coaster one is a part with a pocket to receive an inlay in my case that would be the body of the coaster the other is the inlay plug that will drop perfectly into that pocketed coaster let's tackle the coaster body first this part will be cut from the bamboo plywood so I'll make sure my settings in the setup panel reflect that the important one here is the stock thickness to start off my design I'll first draw a 100 mm circle on my canvas and move it to the lower left corner where my origin is this will be the outer profile of the coaster now I need something to inlay I'm using a nuca cola logo because my boss George is a big Fallout fan and I'm trying to Curry favor here but in general the best candidates for vcarve inlays are designs that have sharp Corners if a design didn't have sharp Corners you could cut pockets to receive match and cutout shapes easily without inlay mode but inlaying a design that has sharp Corners now that's a flex and it's what makes detailed vcarve inlays such a special and compelling use case for cnc's I'll drag my SVG design elements into the canvas delete any extraneous vectors and then group the features so that they stay together I'll use the scaling tool to size the nuca cola logo to fit nicely inside this circle and using the move tool I can then position that logo in the center of the coaster although because of the shape and positioning of the swoosh in that logo I think nudging the whole design a millimeter off center actually looks more natural that way everything looks more evenly spaced around the edges now I think we're ready for cam the tool padding for the coaster blank is relatively easy first I'm going to throw an advanced V carve tool path on the nuc cacola design the depth of this Advanced V carve will be 5 mm I will also take the check boox to enable area pocketing in case you're wondering what settings I would use for this project here they are depending on your material and machine configuration you might be able to push your CNC faster or you might want to slow things down for maximum accuracy if you have a lot of really fine delicate features in your design bamboo plywood is generally pretty tough and stable so I'm not super worried about it chipping out I don't need to Baby the material by taking super shallow step Downs I'd consider these settings pretty safe and also usable for most common Hardwoods I will also note that in this example for this particular operation the e in endmill isn't actually used for pocketing since it's too large to fit in this geometry but area pocketing does still need to be enabled so that the V bit will go to work where the pocket bottoms out to cut out my coaster I'll be applying a contour tool path to that 100 mm diameter circle in my design same cutting parameters for the 8in endmill that I mentioned before and I want this tool path to go all the way to the bottom of my stock material this is what the simulation for the coaster looks like we'll see how closely it matches the machine piece when we get to the shop I'll export my tool paths to a separate file and do some housekeeping before working on the inlay plug I think it's easier to keep my master designs in one file so I need to make sure I'm staying organized to avoid any confusion later I'll rename my default tool path group as coaster tool pads and then disable it to clear the Slate so to speak then I'll make a new group for inlay plug tool paths which will populate shortly clean up complete let's go back into the design workspace the inlay plug will be machined from Walnut so I'll edit the thickness settings in the setup accordingly the most important thing you need to remember for vcarve inlays is that the inlay plug needs to be mirrored otherwise you're going to have an unwelcomed educational moment at your CNC when things don't fit I'll copy and paste my nuca Cola design use the horizontal mirror function to flip the logo and then move it aside while I do a little more cleanup with that mirrored logo still selected I'll open up the layers tool box hotkey L if you're into that kind of thing and create a layer just for my inlay plug then I'll click on the options button that dot dot dot next to the layer in question and move my mirrored design to that layer I'll also activate this layer so anything else I create is automatically assigned to this layer now I can hide my original coaster design which is on the black default layer layers can be just as useful for organization as they are for assigning tool pads so if you're not using this feature already I highly recommend giving it a try to turn my design into a VC carvable plug we need to draw an additional boundary that encapsulates the design this could be as simple as a rectangle or Circle drawn around the design or as streamlined and optimized as an offset Vector why do we need to do this well the inlay plug needs to be the opposite or inverse of what was originally machined it has to form a positive TW into the negative that is the pocketed coaster drawing a boundary that encompasses Your Design causes the tool pathing algorithm to flip it will machine around the design instead of Machining inside the design that creates the matching shape that will fit into the coaster for the sake of minimizing the amount of material I will need to vaporize with my CNC I'll create a streamlined offset Vector 6 mm outside the backwards nuca Cola logo taking care to also clean up any Vector bubbles that are formed in the process now that I have this I can go make a tool path I'll create an advanced vcarve tool path and select my design and its boundary you can do it by selecting everything on your canvas first or selecting it by layer either way is valid I'll enable area pocketing and use the same cutting parameters as before the last section of the advanced vcarve dialogue is where things will start to differ this time we'll check the box to enable inlay plug mode when you do that the depth parameters and the helpful diagram next to the fields will change what these parameters are I think is pretty self-explanatory but I'll give you my thought process about how to pick these values my coaster has a pocket that is nominally 5 mm deep the plug I make should not exceed this depth and to account for space where glue might pull and accumulate it would even be beneficial to shorten the plug to create a small artificial gap between the bottom of the inlay and the floor of the pocket what has worked well for us in testing is to specify the plug depth to be half a MM less than the depth of the pocket in this case that would work out to be 4.5 mm the top Gap is the nominal flatto flat distance between your pieces you'll want some amount of gap for two reasons one is to allow for glue squeeze out you just need a little bit of space for glue to escape when you clamp everything together two is because this gives you some margin for error if your pocket gets machined a little too big or your plug is a little too small you have some extra material to wedge into that pocket there is an optional third reason which is that if you want to cut off excess material from the inlay with a band saw having this Gap will make it much easier for you and the saw in our testing a top gap of 1 or 2 mm has worked out pretty well that's all you need to machine the inlay geometry to separate the plug from the rest of its stock I'll manually select the encapsulating vector and throw a contour tool path on it that goes down to the bottom of the stock here's a quick tip you can use the variable T to represent the stock thickness and you can also evaluate basic math expressions in these fields as well so if you ever think you'll want to run a project again on a material that's a different thickness using variables in your tool paths can be a great timesaver and help you avoid mistakes like forgetting to change your cutting depth you'll be able to measure your stock plug its thickness into your project settings and your tool path depths will all be automatically updated okay that wraps up the tool path for the plug we can double check the simulation but I think we're ready to do some Machining at the shapo 5 I'm going to start with my bamboo plywood I'll be using double-sided tape for work holding since I'm too lazy to use clamps and tabs this is also partly why my speeds and feeds aren't as aggressive as they could be even though I have a big fat 80 mm vfd spindle on this machine I don't want to accidentally rip the material off the table and send it flying after setting my origin and loading a v bit I'll let my coaster tool path do its thing remember this design was too narrow for an 8in endmill to effectively do the area pocketing which is why we're jumping straight into the VC [Music] carving then with a quick swap over to an 8 in endmill I'll liberate my coaster from its stock one thing to note here is that I've substituted an Amon 8in down cutting endmill for the 102 endmill I'd normally use stray bamboo fibers can be pulled like a thread for quite some distance across the plywood face so on the Cosmetic side of this coaster I want to do everything I can to minimize the fuzzies this is where a down cutting bit shines using a synthetic bristle brush can help remove any fuzz in The Valleys of the vcarve and some fine grit sandpaper will Shear off any stray fibers on the top surface before they can cause problems this looks good or at least good enough I kind of messed it up by aligning my origin and thus my coaster too closely to the edge of the material there's a small flat on the bottom of the coaster but thankfully it's almost impossible to notice unless you're looking for it now for the inlay plug I'll start by securing my Walnut and setting my origin at the corner 8in endmill goes into the spindle and We're Off to the Races then we switch to the [Music] bit and then for Speed and because this material is thicker than half an in I'm using a 251/4 in down cutting endmill to separate my inlay from the stock I can push this cutter a little harder than the e in un Mill brush off any fuzzies and we're good to go it's always good to do a preliminary check matching the coaster to the in lay these should fit pretty tightly without any noticeable play and with a small gap between the bamboo and walnut faces so far so good now for the real test when making an inlay you want to make sure you thoroughly coat every mitting surface with glue this will not only ensure your plug is secure and evenly supported underneath but it will help fill tiny gaps and voids and then once you join the pocket with the inlay clamp the heck out of it the more pressure the better because you'll get a cleaner looking inlay with imperceptible small gaps now the amount of force involved in this step as you wedge the inlay into the pocket and squeeze out excess glue is pretty significant this is one reason I'd recommend cutting your inlay plug out of material that's at least half an inch thick so the backing material has enough strength to hold together or if you really want to be frugal and start with a thinner piece of wood put an extra piece of wood behind the plug to help distribute the force evenly when you're clamping depending on the glue type your set time may be different but we'd always recommend letting the inlay sit overnight before you try to cut away the excess material speaking of cutting away that material to machine away the plug I'm going to do some quick math my coaster plus inlay will be my stock thickness here and I want to cut down until I'm just above the surface of the coaster I want the inlay to stand just a fraction of a millimeter proud for cleanup referring back to my original coaster design in the design workspace I'll draw a generously oversized rectangle over where my nuca Cola logo is this just needs to roughly aligned to where my inlay plug is also just to make sure this rectangle doesn't interfere with the inlay plug Machining make sure you put this Vector on a different layer going into the tool pathing workspace I'll select this rectangle and apply a pocketing tool path with the appropriate depth to achieve the desired result at the CNC I'll start by taping down my Puck of wood and eyeballing the front and leftmost points of the coaster this doesn't need to be a super precise zero at least in the horizontal plane you'll want to get your zero height pretty close to exact though then I'll run my plug removal program and wait anxiously for the final inlay to reveal [Music] itself now this looks exactly like what I want and it avoids two pit Falls that can create more work for you the first is that if my pocketing tool path had touched the coaster the endmill could leave tool path marks on the bamboo even if you have a perfectly trammed spindle a spinning endmill can impart swirl marks into the wood fibers that you'll have to sand out the second is that when you inevitably do sand your inlay having both inlay and plug at the same depth will create mixed dust that dust can work its way into the wood fibers and pores reducing the contrast you get you can try to vacuum that dust out but it will never be perfect in this example you can see both those flaws ideally I would have wanted to only sand away a walnut and stopped as soon as it was flush with a bamboo but I wanted to try and sand away as much of the tool pathing marks as I reasonably could and now there's some bamboo dust forever stuck in the Walnut grain an alternate way I could have approached removing the excess plug material would be to hack a 3D roughing tool path in carbide create Pro I can trick create to produce a surfacing pass parall to the Natural grain Direction This hid's tool path marks much better and requires much less sanding to make the face of the coaster Flawless that's how I got this coaster to look perfect even though my surfacing tool path touched the face of the bamboo on my Fallout inspired coaster though things are looking pretty good after a little bit of sanding all that's left to do is apply a coat of finish and there we go one vcarve inlaid coaster ready for service in whatever post-apocalyptic Saloon you frequent so to summarize in order to create a vcarve inlay you need two designs the first design will be Advanced VC carved directly into your stock as a pocket the second design for the plug needs to be mirrored and then have a contour drawn around it then you can apply an advanced vcarve operation selecting inlay plug mode in the tool path options beyond that you should already have the skills you need this capability is something we've been really excited to roll out because it has so much potential in artistic applications and we think this this adds a lot of value for CNC Woodworkers we hope you give it a try and look forward to seeing your results if you have any feedback about it you can share it in our Forum thread which I will link in the description below Oh and before Kevin finds out I snuck back onto the carbide YouTube channel I do have one Advanced tip to share regarding carbide create you may have noticed that I don't show myself setting a zero height at the CNC that's because in many cases I prefer having my zero set at the bottom of my material this inlay project features multiple sets of tool pads that all have to start at different heights instead of setting a zero height every single time I can gauge the surface of the hybrid table once and never think about it again and to account for the thickness of double-sided tape I can just use a piece of paper folded into thirds when I touch off on the hybrid table it gets me a Flawless depth of cut every time where I just barely reach the tape this workflow may not be for everyone but it's how I prefer to work and regardless of your preferences whenever you load a new or old program you should always look at the preview as a gut check are my cuts above my origin or do they go below the origin should I set my zero at the top of the material or at the wasteboard because past you might have specified An Origin differently all right that's all I have for this video good luck and have fun Machining folks [Music]

Channel: Carbide 3D

Views: 5,856

Keywords: Carbide3D, CNC, Shapeoko, Carbide Create, Carbide Motion, Technology, Machining, Nomad 883, Nomad CNC, Nomad Pro, Desktop CNC, CNC Router, Digital Fabrication, Nomad 3

Id: 241eTfM1Dss

Length: 18min 1sec (1081 seconds)

Published: Mon Jul 01 2024