Some info on cnc tool changes and combo cnc/laser projects

@brent113 asked me a few questions about my process for cnc & laser. It was in response to some of the pieces I’d posted in this thread: Multi tool projects
We thought it would probably be good to share some of my answers and methods and some tips. Hopefully it will be helpful.
This information should probably be considered intermediate to advanced. At some point I may make a guide to using Fusion 360 with svg’s and creating tool paths, and also using Easel by Inventables, but this assumes you already know how to do that.

These are the two tap handles that I created that use pretty much every trick I’ve learned:


The only thing they didn’t use was carving from two sides:

Here’s the discussion:


brent113
Hi Steve, that turned out so well that I wanted to ask your process for doing tool changes in the spindle and also CNC to laser changes while keeping everything lined up. Is there a special process you go through?

Most of my tool paths are in Fusion, but I’ve found for some v-carve (recessed) lettering that Easel is easier. In this case I used Easel.

When I post process and create a toolpath I make sure when I name it I include pass #, bit size/type, path type. So for this it would be something like Holy_Pass1_qtr_adapt.cnc or Holy_Pass4_1pt5ball_pkt.cnc. Helps to keep from using the wrong tool. When you’ve got 7 or more passes on some things and sometimes different passes using the same tool it helps.
On the Holy Growl tap handles since it’s two pieces I ended up with 8 passes each on handle and logo:

(you can see that I’m not always good at remembering pass #, oh well. Another reason why I have tool listed too)
The lettering was created in Easel and uses a 30º v-bit. I actually used my SM to cut out both a pocket and a dowel to strengthen the attachment of the two pieces.

Depending on the object I’ll either use center origin or bottom left. I generally prefer center when I’m doing combo laser/cnc but in this case I since I used Easel it uses bottom left so it was easier to keep that consistent.
If I’m doing something on two sides (flip over) or multiple pieces, I’ll use lower left and use a guide that I cnc’d out of a piece of 1/2" ply that I’ve attached to the workpiece:


(I actually created a path and used SM to cut it out. That way work origin is exactly the same then for workpiece.)

Tool height I set using the calibration card as I would for 3d - pull, no push. I’ll pick a point that I know won’t be carved to set the z-height - same as work origin if possible but if not off to the side. I’ll make a circle around that point with pencil or sharpie just so I remember. (I try to always move 10mm increments so it’s obvious) I also make sure to take a picture of work origin on the display in case I mess it up. (It’s easy to hit set work origin when just meaning to do Z) Then good to go. Just be careful after changing bits not to hit “go to origin”. If you’ve got a longer bit you’ll crash it into the piece.
I usually just use the cnc bed for any laser engraving I’m doing on a cnc piece. Even when I’ve gone over the edge it doesn’t do much to the bed since it’s far enough away. If I’m doing laser and then more cnc I don’t want my origin to change. I’ve found the repeatability on my machine to be good enough that I don’t worry about swapping toolheads.

For this piece, since I was doing the laser last and the faces were angled, I had to remove the pieces anyway. In this case I needed to protect the faces that weren’t going to be layered. I used a couple of pieces of scrap plywood and attached them with blue tape and hot glue. In this case I had created the graphic to the right proportions (a little over for safety) and made sure the dimensions matched in Luban. Sometimes I’ll use a piece of masking tape to mark the center and position it that way. In this case it was easier to use run boundary to watch the path of the laser and adjust the work piece. So for the two tap handles I ran four passes of two different graphics.
Another trick I’ve found for lining up laser on a cnc piece: Tape a piece of thick paper on top of the workpiece. If you have any raised or recessed features you can use a pencil or crayon and do a rubbing. Run the engraving pass at low power so that it marks the paper but doesn’t cut through and then measure and adjust your origin until it’s where you want it.

One thing I’ve found in milling some of the thicker pieces that have a lot of bit contact and are going across some pretty tough grain (like the circles) is that I make sure that I set it to conventional milling (not climb) so the path is how you would use a hand router. I also found that it’s a good idea to run the contour path that cuts it out (use tabs) first. This is where bad stuff, chattering, gouges etc., is most likely to happen. So get this out of the way before you spend hours carving something. (You’ll see that in the numbering of my tool paths I have contour as my final passes. After wrecking a nearly finished logo piece was when I decided to always do this first)


brent113
Thanks for that, that’s great. Just recapping some of the points that stood out to me:

  1. 1 file per tool per pass.
    Would there be any benefit to adding the gcode commands into the controller for a tool change, so it can be multiple tools and passes per file? This is something I’ve been thinking of adding, seems like it would be nice to do tool changes and then resume.

At first I thought that would be the case and stupid it didn’t allow me to pause. But now having worked with it I think it’s better. A lot of times after observing the first pass I’ll change something slightly and redo the next pass.
Also makes me think about what bit I’m changing to. It would have to give me instructions like “Insert 3.175mm ball mill”
Takes a little more time to do but pretty insignificant in the big picture.

  1. When you do multiple tools and the tool stick out changes, it sounds like you don’t reset work origin. Are you still setting a new Z work origin? Or is there a way to adjust for tool stick out that doesn’t involve changing any of the X Y or Z origins?

I change Z origin. It’s no big deal and far easier than trying to measure the tool length and compensate or get it exactly right (as soon as you screw in the collet it may change length). Just pick a place to use to set and stick with it. (although I haven’t had any problems when I’ve used center and then realized I’ve carved that part away and had to set it somewhere else)

  1. Sounds like you did the laser in a flat orientation, and that’s what the plywood was for. Before that though, when those angled faces were milled, were those done with angled toolpaths with the work in a flat orientation? The surface finish came out great, and it seems there should’ve been stepover marks from the angled passes - you must have sanded those off prior to lasering.

Milled angles using ball mill with 1/3 bit diameter stepover. Didn’t need to re-orient them at all. They actually come out remarkably smooth. (sometimes the pattern is actually pretty cool) Light sanding, 80, 120, 220 and they were gone. For laser workpiece needs to be repositioned to be horizontal to laser path. I have a panavise head that tilts to allow leveling.

  1. Milling the tabs first is a good tip. Do you leave pretty hefty tabs so the piece doesn’t vibrate? 1/2" long by 1/4" tall spaced every 4" or so?

Depends on the wood. With hardwoods like oak, maple, walnut it doesn’t take much. On the 100mm circle of the tap handle I used 4. 3mm high by 4 or 5mm wide. If you haven’t quite cut through be careful and trim off excess using a utility knife or chisel. Made mistake of trying to snap off and took chunks out of edge.

Hopefully this is helpful. Feel free to ask any questions or let me know if I need to clarify something.

-Steve

11 Likes

This is a great summary!

I can only confirm your findings. Those are very similar to my own conclusions. For example I very much prefer the different files for different passes as well. Pausing and changing toolheads would be more complex.

I too take pictures of the screen with where the original work-origin was set as I’ve made that same mistake :slight_smile: of accidentally resetting it when I only wanted to change the z-axis.

Some personal additions:

  • For setting the z-height: I use a small piece of conductive tape (copper or aluminium tape, the last one you can get pretty cheap, it’s often used to seal HVAC tubes) that I paste on the spot of the workpiece I use for the z-level. Typically close to the border so it hangs off on one side I i can connect a small alligator clamp to it connected to my mulitmeter. The other one connected to the drill bit. Set it to beep on zero resistance and lower slowly until it beeps.
  • When you do a run boundary: always go up a few cm before you do so. First time I usually also make sure that the drill bit is higher than the highest clamp. Just to be sure. Run a second time lower when you’re confident it won’t hit anything.
  • After setting the z-axis height for the work origin and starting the job: always raise the toolhead again high enough that it won’t hit anything. Otherwise it will just move horizontally and a small uneven-ness in the surface of your workpiece could cause a scratch, your bit breaking or the linear module skipping steps
  • If you won’t need to reposition your same workpiece on the table, a really simple way to mount it is as follows:
    • put some strips of painters tape on your wasteboard.
    • put some strips of painters tape on the opposite side of the workpiece (aligned with those on the workpiece
    • use some superglue on the painterstape (not too much so it doesn’t go over the sides of the tape)
    • stick them together and keep pressure on for 20 seconds.
    • by the time you’ve set your work-origin you’re ready to mill
  • “tram” your bed and linear modules in a repeatable way.
    • You can do it properly like @brent113 does here: Carriage Tolerances - Unusable Over Distance >75mm From Center - #34 by brent113
    • or the way I do it. Before starting a milling project: when the power of the machine is off: raise the x-module completely to the top (pull/push it up as far as it goes on both z-axis) & pull the bed completely to the front as far as it goes. That way you know both are aligned (not needed for the x-axis as there is only one). Maybe they are not aligned perfectly, but at least it’s consistent and repeatable. If (like me) you’re a bit too aggressive with the speeds and feeds in your first projects get something stuck. You can make sure this way that you can get it back to the same alignment as before. (just repeat the above procedure)
  • Make sure your bed and x-axis are aligned & parallel to each other. It’s not necessarily a big problem for some projects and if you’re cutting the top layer away anyway. Bu I’ve done a 2-sided project recently and in that case it’s really important. The easiest way to achieve this is to mill away the top 1mm of your waste board.
  • Always make sure you can turn the machine off immediately (kill power!) Again, for the above situations. It will happen at a certain point in time, especially if you’re new to cnc (like me)
  • Use some form of dust collection. I’m using this setup and it works really well: CNC vacuum (too much wood dust) - #8 by brvdboss I did put in a (3d printed) cyclone dust collector in between and that works really well. (using it with a standard home vacuum cleaner at the lowest setting and it works really well for me)
    • When using a setup like this: make sure you don’t run the attachment in your workpiece or clamps. I’ve made the mistake of doing a run boundary without it being mounted and then hitting clamps when actually running the job.
  • For the toolpaths:
    • So far I’ve preferred speed over depth of cut. Depends on the material obviously (in my case mdf mostly so far). When in doubt, I prefer a less deep cut and more passes at a potentially higher speed. The advantage is:
      • smaller risk of your bit getting stuck in the material and breaking
      • If you want to go faster at some point, you can just increase the speed on the touch screen. Going slower with a deeper cut doesn’t work that well usually, and you could end up “burning” the wood in stead of cutting it.
      • A nice side effect of bumping up the speed: the travel is between different spots goes faster as well. With the free version of Fusion the travel speed is rather slow (one of the limitations of the free version)
      • Some materials are harder/softer at different depths (again mdf: hard first mm, softer on the inside). That’s when I usually increase the speed a bit after those first layers.
    • When starting: start slow the first time with a new material/bit and adjust speed based on what you hear
    • When I was starting I often set the work-origin 3mm higher and watch it do a first layer before I started at the real hight. Just to get a feeling for it.
  • I’ve tried some pcb milling as well (tiny 0.2-0.6mm bits). If you want to avoid breaking too many bits: get a sheet of xps-insulation foam and experiment on that. It’s really easy to machine and getting speeds or depths wrong won’t kill your tools. Do make sure to have a vacuum, those things fly everywhere.
  • For two sided milling: I use the “dowel” method. Create a toolpath with 4 holes around your workpiece. I’ve cut 20mm segments of a steel rod (diameter 6mm). Machine holes the same size in the wasteboard (or a sacrificial plate in between). Machine holes in your workpiece (outside the border of your actual resulting piece obviously). Depending on the thickness of your stock you can do that in one go or to do it in two passes. Put the metal dowels in. Machine one side. Turn your piece around, put it back on your wasteboard using the dowels for alignment and machine the second side.
    • In all honesty, I didn’t get perfect results on that yet. There was some misalignment still, but it looked like there was some torsion on my vertical axis. I still need to do some more testing with this.
    • The final cutout (which I did do last in this case) I thus did from one side to avoid that misalignment. (that way you can’t really see it with the naked eye. it’s really limited, but still it avoids the need of sanding it away afterwards)
5 Likes

Thanks for the additional adds. I agree and have tried or do almost the same on pretty much all your other points.

Thought about doing this too. Just haven’t gotten around to it. Would definitely be quicker and more accurate.

This works well. Had it release on some heavy oak once. Not sure if it was pushing too hard or didn’t glue well enough or didn’t wait long enough. Spray accelerator on one side and use super glue on other to speed up.
You can also use hot glue gun with blue tape. Tape bed and lower edge of object. Glue where they meet on bed. Either a fillet or a glob every so often and on corners. If bit hits glue it doesn’t hurt it.

Haven’t need to do this on mine. As long as I go home (especially if I’ve run into something) I’ve been fine.

Definitely!!! I have a switch I hardwired to do this. (The power supply uses a standard power cable. You probably have an extra one lying around. Standard light switch and electrical box and you can make one.)

Haven’t done this specifically. Partly because so much of the stuff I do needs every mm of clearance. I use shop vac every so often (have a cyclone attachment to keep from killing bags). Fan on enclosure running vented to outdoors keeps dust from leaving enclosure.

Great tip! I do this often especially with programs that are new or I’m tweaking g-code that I don’t totally trust. Or with multiple programs.

Haven’t tried this yet. For a couple things where I’ve only had one side (or no sides) that were flat, I drilled a small hole all the way through the piece and used that to set my work origin. When you’re doing clearing and leave stock, it’s easy to see if it’s out of alignment and adjust before you do the final pass with your smallest bit.
When I use the workstop with lower left origin, I flip the work piece over and turn it 90º so that the same corner is always at the origin point.

-S

1 Like

I’ve gotten a power strip with an on-off button for each outlet on it. That’s mounted at arms length against the wall in front of my workspace and has all “dangerous” devices plugged in. the SM, my soldering iron etc. They also light up, so I notice it immediately if I turn off the lights when I’m done if I left something on unwillingly.

But I agree it’s easy enough to make yourself. Definitely a necessity.

I once ran in to the bed quite hard (going down, being impatient and tapping the screen too fast, or in another case forgetting it was on 10mm in stead of 1mm :see_no_evil:. It was almost completely on the right and there definitely was a few mm difference between both vertical axes. Home didn’t fix it and when I then pulled it to the top completely, there was still a difference. Meaning it was aligned a bit different form the start. So now I’m rather safe then sorry and always do this before I start a cnc job.
It’s not necessary, but it sucks if you turn your workpiece in scrap after the machine has been milling for 8 hours :stuck_out_tongue:

That’s a good tip too! I now just flip it over.

It sounds like you just line up the origin for Laser passes manually? Have you tried finding an offset between the laser module and CNC modules so you can just compute the laser origin from the CNC origin? I haven’t tried that yet, but it seems like it should be the ideal solution.

Considered it but never ended up doing it.
Main reason is that file dimensions and shapes usually end up being different than cnc. By the time I figure out and adjust everything in whatever program I’m creating my artwork for engraving or laser paths it’s just easier to do it manually.
-S

Great thread! I’m just starting out with CNC (already managed to break two bits this weekend), but I like the idea of being able to do multiple tool passes. A couple of questions:

-I’m assuming this means that the z offset is independent of the work origin (x,y)? I didn’t realize that it was separate coordinates-neat!
-I gather that small irregularities in the surface (I was just using bits of scrap to test) are going to be an issue, so are you guys doing a first “facing” pass on any pieces you mill?
-It looks like you’ve got some larger bits in there for toolpaths and roughing out the bigger sections. Are you able to use something bigger with the A350? It looks like it’ll take anything with a 3.75mm shank, but I wasn’t able to find anything on Amazon with a larger head and smaller shank.

New bits are on the way, so hopefully I can try some of this out in the next week or so.

1 Like

It’s all tied but you can set each individually before running the job. This works out nicely with the laser sometimes. Like if you’re doing a cutting board and want the graphic to be a certain distance from the corner you can line up the dot on the bottom edge then move up a specific amount and set the y. Repeat from the side for x.

All depends. If everything is going to be cut away anyway, than why bother. But sometimes. I have a few .5mm milling passes of various sizes saved as gcode.

You can get a set of er11 collets that will allow you to use up to 1/4"/6.35mm shank.

-S

Thanks! That really helps. Started looking at the ER11 collets on Amazon. When I was looking for bits, I got the impression from other posts here that looking for something marked HSS (High speed) was all you really needed to worry about. Any pointers on what to look for otherwise? Any suggestions for something good to check out for a larger “first clear pass” bit to use with an A350?

HSS is a type of tool steel, as opposed to carbide or other metals cutters are made from. HSS and carbide will both work.

HSS supercedes high carbon cutters, there’s some interesting history there from 1940s machining technology.

As far as types, this kit (which you don’t need) has a nice selection of shapes and sizes you can reference off of: https://www.amazon.com/Freud-Router-General-Purpose-87-208/dp/B01LX903DH

It’s the kit I use, but you definitely don’t need to spend that much. A variety of straight and V cutters, some tapered ‘pointy’ bits for fine detail, whatever you need really.

Edit: Thanks SDJ, I also use Whiteside bits on my router, they are very high quality. Also Rockler makes (relatively) inexpensive good quality router bits, likely would work for the SM also. These guys.

Carbide is harder than HSS and will stay sharp longer. HSS tends to be cheaper. For the type of use they’re going to see on an SM it probably won’t matter.

There are a lot of choices and price ranges. Amana is widely regarded as the best but with a price that matches the reputation. For larger bits and final passes I really care about I’ll spend a little more. I really like Whiteside and CMT for value. They perform great and don’t break the bank.
For smaller bits, since they break easily and there is less to stay balanced I go with cheap. I’ve really liked the HQMaster that you can find on amazon and ebay. But they’re all probably made in the same one or two factories.
For flattening most stuff and first clearing passes I use a 1/4" downcut bit.
If you want to surface a large surface (like your bed) you’ll want a spoil board cutter I went with a Whiteside: https://smile.amazon.com/gp/product/B071748JQN/ref=ppx_yo_dt_b_search_asin_title?ie=UTF8&psc=1
You can find cheaper but with the diameter it’s spinning I wanted one that I could trust to be balanced. Need to use small step-down - .2mm to start.
As far as other things to look for there’s a whole world of choices as far as number of flutes, profiles, upcut & and downcut etc. This will help get you started:
CNC Router Bits – A Simple Guide | All3DP

-S

@brent113 and @sdj544 already mentioned all the important stuff.

It all depends a bit on what you want to be doing. What I did for myself was just order a bunch really cheap bits from the well know chinese websites. the SM2 is my first cnc type of device and I knew I would want to get some practice first and learn what type of bits (and sizes) would be most useful.

Now that I had some practice I’m getting a feeling of which types of bits I’ll be using for most of my projects and what’s most convenient. For example, there are often a lot of sets out there that have for example every size between 2 and 3mm with 0.1 increments. You usually won’t be using all of those.
Why not? Let’s say you’ve got one of those sets, in the middle of a job your bit breaks (or most likely at the start :), anyway, your bit broke and/or isn’t sharp anymore). What will you do? Just insert another one, maybe adjust your working speed and continue.
If you insert another size, you’ll have to regenerate your entire toolpath for the new bit size vs just insert the new bit and restart the job.

So you end up standardizing on the more common sizes anyway. And in the end that often means the biggest sizes you can use at the highest speeds (i.e. what results in the shortest time to finish the job) or what requires the least amount of tool changes.

As you go you’ll build up your list of favorite sizes and then you can spend a bit more on better quality bits that you’ll use more often.
On my list so far:

  • a surfacing bit
  • a 6mm bit (with larger collet) for larger clearing passes
  • a 3.175mm bit (which fits in the standard collet)
  • a number of 0.4 or 0.5mm bits for making pcb’s and 0.8mm for through holes

So far in my experience my cuts are not deep at all, so I tend to prefer downcutting bits as they result in the best looking edges from the top.

But in general it mostly depends on what you’ll be using it for. Do you intend to be making v-varved inlays or are you doing really fine detailed carvings etc you’ll need v-bits etc.

I’ve been using them for at least a decade for woodworking. Absolutely love their chamfer bits. U.S. made too if that’s important to you.

Should’ve included my source for good bits. Great service & prices and best of all fast and free shipping: Cutting solutions tailored to your particular needs!

-S

Hope you guys don’t mind me adding to the thread with a question but I’m completely new to CNC and wanting to attempt to set up multiple passes for a design I’m working on that’s 240mm x 240mm x 26mm. I started cutting it with a carving V bit but realised it was going to literally take days so wanting to attempt to cut the rough larger depth out before going over and finishing up with the carving bit.

I’m trying to wrap my head around how you would set up the second pass to not have to spend ages going through the same depth so it can get straight to cutting the remaining material. Any tips would be super useful!

Edit: To add to the bit discussion, after snapping the flat end mill bit that came with the SM I invested in some Tungsten Carbide ones and they seem to be doing well!

I’m sure this applies to CNC as well. I followed some advice regarding router bits when I just started: buy a set of cheap bits, I got a 15 piece MLCS bit set. They don’t last very long, but when they get dull or wear out then you replace them with a Freud, Amana, Whiteside, etc. Then you only spend the bucks on bits you actually use.

I have a Whiteside 1-1/4" spiral compression bit that was a splurge, but good lord I use it for everything now. It’s incredible.

1 Like

What software are you using? In Fusion 360 it’s a standard feature to have multiple toolpaths that follow each other. So you have a first roughing pass that leaves 0.5mm for example and then you go in with the best bit (ball end, v-carve, smaller diameter) that you need to clear out remaining parts. So the software that generates the toolpaths takes into account what’s already milled away.

Luban does not support that.

Ah, yes. Well, I was using Luban, though I was thinking it might not support it! I’ll have to give Fusion 360 a go! Assuming you guys are generating the G-Code with other software then loading onto the Snapmaker directly and running?

have a first roughing pass that leaves 0.5mm for example and then you go in with the best bit (ball end, v-carve, smaller diameter) that you need to clear out remaining parts

That sounds like exactly what I’m looking for, thanks for the info! How do you know to change the tool with SM? Do you load multiple g-codes and the additional ones already know where/what to cut already using the same work origin and you just swap the tool between passes?

You should read this whole thread.
-S

1 Like

Ahh I missed it, you’re right. Multiple files, one file per pass. Got it!

Thanks everyone for the suggestions-lots to look into! I ended up ordering a bunch of replacement 1.5 and 3.75mm bits. Bought cheap multipacks of each because they break easily, and I can see them wearing out as well. See how those last. Next might be a couple of larger ones assuming that I want to be able to do things faster.