| Official Luthiers Forum! http://w-ww.luthiersforum.com/forum/ |
|
| RhinoCAM setup for milling a neck http://w-ww.luthiersforum.com/forum/viewtopic.php?f=10106&t=37686 |
Page 1 of 1 |
| Author: | Ken C [ Mon Sep 10, 2012 6:57 pm ] |
| Post subject: | RhinoCAM setup for milling a neck |
I need some help from any RhinoCAM users out there. I have the basic version, and I am trying to mill an acoustic neck that I have already roughed out on the bandsaw. However RhinoCAM gives me rectangular stock, and I can't find a way to limit the milling region on the Z axis, so I end up milling air until the bit works its way down to the actual neck blank. I can define regions that limit the X and Y movement, but not the z. Am I missing something? The only way I can see to make this work is to split my neck file into two separate CAD files and machine the heel in one and the neck in the other. But I have to think there is an easier way. This is the stock I get from Rhino: Attachment: Stock.jpg But rather than mill air to get down to here, I'd like to start from here: Attachment: Roughed.jpg Thanks! Ken |
|
| Author: | turmite [ Mon Sep 10, 2012 7:31 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken I don't use Rhinocam since I resell and support Madcam...  ....but there should be a region curve command and a clipping plane somewhere for you to limit the amount of air time. Madcam allows you to use a stock model like you would have bandsawn out and that automatically limits the roughing and finishing passes within that model. I still have to use region curves and clipping planes on some programs. Hope this helped a little. Mike |
|
| Author: | Ken C [ Mon Sep 10, 2012 8:31 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Thanks Mike. Yeah, I agree, there should be! I just can't seem to find it! It's probably something stupid easy that I have simply overlooked. Ken turmite wrote: Ken I don't use Rhinocam since I resell and support Madcam...
....but there should be a region curve command and a clipping plane somewhere for you to limit the amount of air time. Madcam allows you to use a stock model like you would have bandsawn out and that automatically limits the roughing and finishing passes within that model. I still have to use region curves and clipping planes on some programs. Hope this helped a little. Mike |
|
| Author: | ballbanjos [ Tue Sep 11, 2012 5:07 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Another somewhat less elegant solution that works well nonetheless is to split the neck model into three parts--the heel, the shaft and the peghead. Build the stock around each of these areas separately, then combine the G code into one file. The neck shaft stock eill be much thinner than the other two. I've done this since my cheaper version of madCAM doesn't support the stock models that the full blown version does (at least I don't think it does). Saves a lot of air cutting time. I haven't tried the region curve option--I'll have to give a look... Dave |
|
| Author: | Andy Birko [ Tue Sep 11, 2012 7:36 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Hmm...here's an idea. Set up a completely different MOP just to get you to your stock the way you want it. e.g., use horizontal roughing but leave a lot of stock behind for your next operation. I got the idea from your original post. You write, "I'd like to start from here" so, start from "here". Put that horizontal roughing MOP in a separate MOPset that you don't post with your cutting code. You'll simply be using that to "prep your stock" for the real operation. Simulated air cuts are pretty quick ![[:Y:]](./images/smilies/smiley20.gif "Thumbs Up")
|
|
| Author: | Ken C [ Tue Sep 11, 2012 8:17 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Thanks Dave and Andy. Your idea Dave was sort of what I was thinking I may have to do, but Andy, my man, you may have that answer for me! I should be able to set up a MOP that mills away the region I will already have removed with the bandsaw. Then as you say, I just post the ensuing MOPs. Simple…and the idea was right there in front of me the whole time. Duh! Thanks gents! Now I can get back out to the CNC again! Ken |
|
| Author: | Sheldon Dingwall [ Tue Sep 11, 2012 9:53 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
I haven't watched an entire Taylor neck carve but it looked like they carved the heel first, then the shaft. |
|
| Author: | Kevin Waldron [ Wed Sep 12, 2012 3:53 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Not sure if your version of Rhinocam has part offset stock, but if it does set it for say .3". You will need to do regions for the various neck parts. If you want to follow the peghead outside you will have to use the 2 1/2 engrave tool to do so, it will follow a taper ....... ( it will be on the line not either side so you will have to draw a line offset from the part the amount of the tool ) Here is a quick video of what we do. This was a proto for a soprano uke that we make. ( The peghead moves in the video some and we knew this but we posted anyway. ) http://youtu.be/7zkj8vekG4o Hope this helps. Blessings, Kevin |
|
| Author: | Bob Garrish [ Wed Sep 12, 2012 4:39 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Sheldon Dingwall wrote: I haven't watched an entire Taylor neck carve but it looked like they carved the heel first, then the shaft. I remember it looking like a flowline from the heel to the headstock when I was there but that was six years ago and both memories and toolpaths are subject to revision over that timescale 
|
|
| Author: | Ken C [ Wed Sep 12, 2012 8:39 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Kevin, thanks for posting the vid! I do have the part offset feature, so I set up my Air MOP to get me down to 3/8" of my part. That should cover my bases  I am not too concerned in getting the headstock profile dialed in with the CNC, but if I can support the face of the headstock well enough, I would like to mill the back of the headstock. I am using a vacuum under the neck and am hoping a 15° degree wedge stuck to the back will work.Ken |
|
| Author: | Kevin Waldron [ Wed Sep 12, 2012 9:03 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken, You will find that the peghead wants to move a lot. We found that in this area if your going to use vacuum you need a little bit more gasket. In the real world getting this lined up perfect everytime is almost impossible even if you use shapers and templates to get the angle the same prior to placing on the cnc.... some how it just never is perfect. The break point index point for any necks that we do is always on the heel side center of nut... everything else works from here regardless of the neck that we are cutting. The other area where there is a lot of movement is the heel. If you experiment a little you will also find that the material will cut better on one side in one direction than the other..... thus some of our toolpathing on the neck. Happens because of tool rotation but this all comes into play when wanting a semi finished neck. Our final toolpaths are at only a 5% stepover using a 5/8" ball nose. In real time me can cut most necks in the 15 to 30 minute time slot not including the peghead ( peghead roughed not finished in the 15-30 minute time slot ). To finish cut the peghead we vacuum the head down parallel with the table with the neck sticking up which is another operation and is sometimes faster with other equipment. We also use vacuum grid and fixtures for necks that we do a lot. Blessings, Kevin |
|
| Author: | Ken C [ Sat Oct 13, 2012 12:32 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Gentlemen, we have success!! I finished milling a neck for a customer's guitar this morning. Man, what a learning curve. I struggled with everything, including software, holding down the stock, bits, feed and speed. What an adventure! I downloaded a version of MadCAM, which allowed me to mill to a custom stock. In general, the software works, but I am not a fan of the interface. For software that integrates with RhinoCAM, it provides no flexibility to auto adjust the tool paths when the part is changed nor can parameters be changed without recreating the tool path from scratch. But it did cut down milling time considerably compared to my basic version of RhinoCAM. I put away the vacuum jigs and built a new jig that allows me to anchor the neck stock to a MDF spoil board using screws. This jig is then clamped to my table. I can remove the neck in progress from the table or the spoil board and still relocate it to its exact position later. This setup holds the neck down firm, so I had no issues while milling the heel. I also put away the 4 flute bits that came with my machine and bought new 2 flute carbide end and ball mills that I ran at 9K RPM and 140 IPM. No more burning sawdust or stock...whew! I have spent a lot of time working through one issue after another. But I have a much better understanding of my machine and the process now. Milling the neck takes a bit over an hour including tool changes. I could probably shorten the process some, but the machine can whittle away while I work on something else. Below are a few pics, which may help someone going down this path in the future. I decided to set up an operation to allow laminating the back of the headstock. Something I had always wanted to do, and with the CNC, I can do it as just another step in the process. The neck off the mill has some minor faceting, but should clean up pretty quickly with some sandpaper. All-in-all, I am pretty pleased with the results. First step was to slot for truss rod and drill locating holes and screw holes. Then using a template of my stock profile, I mark the neck blank then cut on the bandsaw and attach the neck to the spoil board that will be clamped to my table: Attachment: Neck Milling-3.jpg Mounting the spoil board to my table: Attachment: Neck Milling-4.jpg First milling step is to mill the back of the headstock so I can laminate: Attachment: Neck Milling-5.jpg The neck is removed from the table and the laminate glued on: Attachment: Neck Milling-8.jpg Using a 1/2" end mill I rough out the rest of the neck: Attachment: Neck Milling-10.jpg I finish up with a 1/2" ball mill: Attachment: Neck Milling-11.jpg The volute: Attachment: Neck Milling-12.jpg I will cut the headstock shape using a template and my laminate trimmer. Ken |
|
| Author: | Don Williams [ Sat Oct 13, 2012 5:35 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
That looks awesome! I've never had the guts to try to machine a guitar neck that direction, I've only tried to do make one on its side. What size spindle do you have Ken? That's a lot of bit hanging down, and I don't trust my spindle to have good enough bearings to handle that can of stress. Looks awesome though, and the results look great. One other question...how are you cutting the other face of the headstock? |
|
| Author: | Ken C [ Sat Oct 13, 2012 6:29 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Don Williams wrote: That looks awesome! I've never had the guts to try to machine a guitar neck that direction, I've only tried to do make one on its side. What size spindle do you have Ken? That's a lot of bit hanging down, and I don't trust my spindle to have good enough bearings to handle that can of stress. Looks awesome though, and the results look great. One other question...how are you cutting the other face of the headstock? Thanks Don. Yeah, the bits are long. I am using 6" for each of the flat and ball mills. My spindle is 3hp, but it only has the ER25 mini nut. I found I could not clamp down well enough on a 5/8" tool, so I went to 1/2". With roughing passes at .25" step over and .125" DOC and finishing passes removing even less material, the long bits worked just fine. I wasn't pushing them too hard. What really makes these long bits work is holding the stock firmly to the table. Once I got that figured out, my anxiety level in using these long tools went way down.  I cut the face of the headstock using my bandsaw then cleaned it up on the sander. It was pretty straightforward and quick. Attachment: Neck Milling-14.jpg Ken |
|
| Author: | Andy Birko [ Sun Oct 14, 2012 9:30 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Lookin' good Ken! Never used MadCAM but I'm sure there's a way we can figure out how to get VM to do what you need it to. Good work on the blends as well. I know those can be hard to model. |
|
| Author: | Don Williams [ Sun Oct 14, 2012 9:55 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken, have you thought about cutting the headstock face first, and having an angled block on the fixture? Seems like this way you could then use your index pins for the fretboard alignment pins as well, since you would be dialing in the nut location perfectly prior to doing all the surface work. Darned impressive either way...that transition at the shaft/headstock is fantastic. What brand/quality is that spindle? Mine's a 2.2KW water-cooled chinese unit, and I'm not sure I trust the bearings to handle that, but maybe it's not as bad as I thought. My collet is only an ER20, so less capacity in general, and I suspect my spindle is less beefy than yours as well. Sharp pit, soft wood...not really much resistance, but somehow my mind wants to think there's more there than there really is. You're screwing the blank to the spoilboard? Wow...you're brave. I just know that if I tried that I would ruin the blank or hit the screw with the bit.
|
|
| Author: | Kevin Waldron [ Sun Oct 14, 2012 1:37 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken, Everything is looking terrific! I agree there are things done faster off the cnc than on, but doing things by hand can't compete when it comes to repeatability. If someone doesn't do cnc then they can't appreciate the problems and the patience that it takes to work out all the details for an acoustic neck. Here is our latest project on the cnc, a Cuatro guitar neck from Puerto Rico. ( takes about 50 minutes to run and about 5 minutes of sanding to dress it up. We cut the truss rod slot and the rough cut out by hand as well as the tenon body joint and drill the tuner side holes by hand rest by cnc. ) Blessings, Kevin |
|
| Author: | Andy Birko [ Sun Oct 14, 2012 2:27 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Don Williams wrote: What brand/quality is that spindle? It's a Columbo...I've seen it....it's totally badass. I spun the bit that was in there and it freewheeled for about a minute... |
|
| Author: | Ken C [ Sun Oct 14, 2012 3:07 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Yep, Andy's got it. Columbo 3hp, but I am not hogging off a lot of material. I may have the HP to do more, but I had trouble holding on to bits. I switched to 1/2" with shallower passes and got a new collet, which solved that problem. With the stock already roughed out on the bandsaw, roughing out the rest with the CNC went very quickly even with shallow passes. Don, The screws were easy, I laid them out in Rhino where I knew I had plenty of clearance. When I made my spoil board, I drilled those screw locations as well. When I cut my truss rod slot, I drill my locating pin holes and pilot holes for the screws. My neck blank then aligns with the pins, I zip in a few screws, and mount to the CNC table. No worries about the stock splitting or hitting screws with the bit. Setting up the blanks takes a couple minutes longer using this approach compared to a vacuum, but my neck is anchored down solid. Andy, yeah, I'd like to figure out how to cut the milling time with RC too. I tried your earlier suggestion, but it wouldn't work consistently. Maybe it's a matter of playing with it some more. I even called MecSoft and they wanted me to spend $5k for their pro version. That is a lot to pay just to be able to model stock as I don't need the other axis features. Kevin, that neck looks pretty nice! Ken |
|
| Author: | Andy Birko [ Sun Oct 14, 2012 3:20 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken, When using RhinoCAM, I've discovered that some subsequent MOPs do take into account the stock model from the previous operations during generation of the toolpath, particularly the roughing MOPS. This only works if you run a simulation though that removes the stock. You have to make sure that you ran the simulation for the roughing MOP and that the stock model is in the roughed state when you generate the non-air roughing toolpath. I've gotten pretty OK with VM so I might be able to figure this out. |
|
| Author: | Bob Garrish [ Sun Oct 14, 2012 4:18 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
I've done headstocks 'both ways' on production necks, both before and after the backside of the neck. On the ones I did it before I'd cut the truss rod slot and the headstock face along with pin holes with the blank flat on the table and then flip it onto a vacuum fixture with an angled area for the head. Alternately, if you have plenty of Z (which a mill does, but most routers don't), I had a vacuum plate which sat high enough off the table that I could stick the back of the headstock to it and face off the front as well as drilling the tuner holes. I've also machined necks on their sides or 'back up', depending on the neck. For electric necks 'back up' tends to save setups without much risk, while acoustic necks are easier to hold and machine on their sides. Holding a neck on its side is more work on fixturing, but the roughing passes sure go fast. I don't think I've ever used screws on a guitar neck, but I did use screws to hold down wooden high-heeled shoe blanks to aluminum plates for hold-down in production. |
|
| Author: | Kevin Waldron [ Sun Oct 14, 2012 6:12 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken, After you do a few of these you'll find what suits you best..... in our case we have a large wood shop and a lot of tools... some aren't even made anymore.... ( being doing reproduction furniture for almost 40 years ) so a lot of what drives our cutting or not cutting on the cnc is what tools we have that would and could do it faster or easier. We've tried all kinds of locations/jigs/fixtures on the cnc and each neck has it own quirks. Andy, Rhinocam/Visual Mill has some quirks one is using the ball nose bit.... you have to fake it off to get it to go below the bottom of your parts Z axis if your using the ball nose ( we set our Z zero at the top of the part ) and want to cut flush with the bottom of the part ( so your ball will have to go below the bottom of the part)..... you also have to overlap toolpaths by some margin to get good clean transitions with the ball nose ... we usually overlap .1 at least on the regions... if you don't.. you get a slight visual ridge using a ball nose bit... using a square end mill none exist..... school of hard knots... Bob, We do cut a few necks at 90 degrees of what most think of as top and bottom..... classical being an example.... but again it presents other problems...... ( some of the pegheads can't be cut this way and the solera style block and the neck want machine clean usually ) with 3 axis you can't do a negative cut as you know...... for the most part less handling of the part means more accuracy and less chance of screw-ups and your index points being correct or often in our case being in the way as we cut. We also have a router and it has 19" of z table height and the table is 5' x 12'...... but I'd agree most don't have the z height on a router. We personally have found straight down to be the best for us with our tools for most necks. Here are some examples......... straight down to back of the neck for the diamond volute and the wine glass volute if you rotate them 90 degrees the volutes just doesn't come out clean.... ( the wine glass was cut without placing the head at the same angle as the table but cut when the neck was cut at the 15 degree angle if you look close you will still see the tool marks ) Blessings, Kevin |
|
| Author: | ballbanjos [ Mon Oct 15, 2012 7:02 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken C wrote: Gentlemen, we have success!! I finished milling a neck for a customer's guitar this morning. Man, what a learning curve. I struggled with everything, including software, holding down the stock, bits, feed and speed. What an adventure! I downloaded a version of MadCAM, which allowed me to mill to a custom stock. In general, the software works, but I am not a fan of the interface. For software that integrates with RhinoCAM, it provides no flexibility to auto adjust the tool paths when the part is changed nor can parameters be changed without recreating the tool path from scratch. But it did cut down milling time considerably compared to my basic version of RhinoCAM. I put away the vacuum jigs and built a new jig that allows me to anchor the neck stock to a MDF spoil board using screws. This jig is then clamped to my table. I can remove the neck in progress from the table or the spoil board and still relocate it to its exact position later. This setup holds the neck down firm, so I had no issues while milling the heel. I also put away the 4 flute bits that came with my machine and bought new 2 flute carbide end and ball mills that I ran at 9K RPM and 140 IPM. No more burning sawdust or stock...whew! I have spent a lot of time working through one issue after another. But I have a much better understanding of my machine and the process now. Milling the neck takes a bit over an hour including tool changes. I could probably shorten the process some, but the machine can whittle away while I work on something else. Below are a few pics, which may help someone going down this path in the future. I decided to set up an operation to allow laminating the back of the headstock. Something I had always wanted to do, and with the CNC, I can do it as just another step in the process. The neck off the mill has some minor faceting, but should clean up pretty quickly with some sandpaper. All-in-all, I am pretty pleased with the results. First step was to slot for truss rod and drill locating holes and screw holes. Then using a template of my stock profile, I mark the neck blank then cut on the bandsaw and attach the neck to the spoil board that will be clamped to my table: I will cut the headstock shape using a template and my laminate trimmer. Ken I cut my banjo necks almost the same way using madCAM--your pictures look very familiar! I use a 6 inch long 2 flute 1/2" round nose bit for both roughing and finish cut--I'm lazy, and have put everything together into one tool path. It works out fine. I also cut and flatten my peghead surface first. This is for two reasons--I don't lay out my index holes until the peghead surface is finished. That way, if I end up having to take an extra pass or two to flatten the peghead (and move the end of the peghead down the shaft of the neck a little in the process), It doesn't make any difference. I always have a consistent distance from the peghead "break" to the fretboard. The second reason is that with banjo necks, the peghead shape is cut perpendicular to the fingerboard surface, not to the peghead surface. I use the CNC to cut the peghead to shape along with the rest of the neck shaping. The downside to doing this is that it's harder to hold the neck in place. I use a vacuum clamping arrangement with one clamp under the fingerboard surface and a second one in a wedge under the peghead overlay. I had to put a "tool change pause" in my G code to allow me to install an additional mechanical clamp on the shaft of the neck prior to roughing the peghead (I cut the heel and shaft first). I don't cut super fast, but even at 200ipm or so, there's sometimes enough torque from the cutter to overwhelm the vacuum clamps and knock the neck off. The mechanical clamp gives me a little extra insurance. There's still just a little bit of wiggle in the workpiece when roughing the peghead, but my finish pass takes a light enough cut that everything works out fine. madCAM's interface works fine once you get used to it, and the toolpaths it generates have always worked out well for me. You're right about parameter changes requiring recreating toolpaths, but you can recreate only the particular toolpath you've changed--you typically don't have to go back to square one. On my laptop, neck toolpaths don't take more than a half a minute or less to generate anyway, so it's never been that big a deal for me. Dave |
|
| Author: | Ken C [ Mon Oct 15, 2012 8:52 am ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
I am still refining the process, and currently I am not cutting the tenon until after the neck is shaped. This gives me one more variable I can move slightly to dial in the nut position. I run my anchor screws up into the areas I will be removing later for the tenons. If I cut my tenon and shape the face of the headstock first, I lose my attachment points. I’ll see how this approach works when I go to cut the tenon. Dave, I have the neck divided into 3 regions, and I use a custom stock, with each region getting three milling operations, that is 9 toolpaths I have to keep track of. If I need to make a change, I have to open the Rhino file, redefine the part, the stock, and the region, set all the cutting parameters for the specific toolpath, then finally generate the toolpath. And as MadCAM does not provide any reference as to what parameters were used to generate the toolpath, I have to keep notes separately. So say I mill the neck, and I decide with the next one that I want to mill the heel with a climb cut rather than a conventional cut, but keep the other parameters the same. I can’t just reopen the file, change the toolpath setting for the heel from conventional to climb and recreate the path. I have to redefine my part, the stock model, the region, and re-select every parameter for the particular toolpath, referring back to my notes to see how I set all the parameters so I end up changing only the cut direction. What would be a 5 second change in RhinoCAM is much more involved in MadCAM, and I risk changing another parameter if I don’t follow my notes carefully. I only have exposure to RhinoCAM and now MadCAM, so I don’t know how other CAM packages operate. You are right, making the changes aren’t difficult and toolpath generation itself is very quick, I just feel that for a CAM package that integrates with Rhino, I should be able to simply tweak a parameter, and the software will regenerate the toolpath, rather than create from scratch every time. Perhaps if one understands well how to set up the toolpaths in the first place, the changes are minimal. But for me experimenting and learning the impact of the changes, I find having to recreate the parameters each time a bit of a hassle. Though I am getting a better feel for the interface as I use it more. Ken |
|
| Author: | ballbanjos [ Mon Oct 15, 2012 4:03 pm ] |
| Post subject: | Re: RhinoCAM setup for milling a neck |
Ken, That's pretty much the same way I go about it--nine toolpaths overall. I don't mind redoing the toolpaths if I make a change, but I do get frustrated with madCAM's lack of parameter reference--if I don't take notes, I'm pretty well back to square one if later on I try to figure out what I did earlier. Still for what I paid for a 4 axis CAM, I'm very pleased. It does a good job with the toolpaths and is easy to use once you get used to it. It's not always straight forward to figure out, and the documentation isn't the best, but Joakim has always been quick to answer questions for me via email. Dave |
|
| Page 1 of 1 | All times are UTC - 5 hours |
| Powered by phpBB® Forum Software © phpBB Group http://www.phpbb.com/ |
|