Hi all, brand new to the forum and excited as I'm planning a CNC Router (likely LEAD 1010) build in the near future. I have a fair bit of experience with CNC, but not with desktop routers. As I'm thinking through what I want to use this machine for, I quick realized that tool changing - specifically lack of an ATC - is something I need to consider. For what I'm doing, I expect to need a minimum of 3 different tools per part, sometimes possibly a couple more. I see it's possible to retrofit an ATC-enabled spindle if one wants to spend the money, but the cost of the parts essentially matches that of the entire rest of the router (and it's probably overkill). I see some "quick change" products designed for (non-CNC) routers, is anybody using something like that? Not sure how accurate those would be with respect to repeatable Z-offset, but seems better than doing it the slow way. Anyway - thought I'd put it out here to see what your experiences are. Am I worried about something that doesn't matter? Is there no real time to be saved with something like this because you have to touch-off with every new tool anyway? Appreciate any thoughts or insights - especially if you've come up with a system or process that works really well for you.
It takes me about 30-40 seconds to change a bit and probe it and maybe 50-60 secs if I need a collet change as well. The question is, how much time do you need to save?
Our Fusion360 post creates a Gcode file per tool. If are using other CAM software then you should do the same. GRBL has no facility for storing multiple tool offsets so you have to probe or setZero each tool after you change it, this cannot be done while the Gcode is running, ergo the need for separate files. So, does the time for tool change matter? depends what you are doing, right? If you are into high volume commercial production with minimal operator intervention, then you need to buy a Datron Cube (-: Otherwise you can minimize tool changes by using fewer tools, and by cutting multiple parts at once like laying out a grid of 8 parts instead of cutting just one, then letting tool1 cut all 8 before changing to tool 2, etc. My process for tool changes using bCNC GUI lets me use some of the built in variables, so I can do a G0 X[xmax/2] Y[ymax/2] to quickly go to the center of the part, then I can probe there and start the cut. If you are using the OB XYZ probe then it is easy enough to probe the start corner as usual, my probe lends it self to probing Z anywhere.
So does the OpenBuilds Probe too, just flip it upside down then its just a flat piece you can lay down anywhere
Good info guys, thank you. My use case would indeed be "production" stuff though volumes would be low. I expect to always be cutting more than one part since carbon sheet is expensive relative to the cost of the product(s) I'd be making. I was imagining the process of changing tools taking significantly longer than 60 seconds. If it's really on that kind of time scale, that's almost nothing relative to the rest of the cut time so probably not worth worrying about. I have and will be using Fusion360 (though I also have Inventor and HSMWorks) so it will probably be G-code per tool (which I hadn't thought about). Because I'll normally be cutting carbon fiber, I intend to add a basin to the top of the spoil surface with some built-in work-holding features. I will try to leave a good spot to touch-off within that, should be quite workable. When I learned to run a CNC mill years ago, we touched off on an 0.010" feeler gauge and set zero 0.010" below that - same concept might work here.
OB post Releases · OpenBuilds/OpenBuilds-Fusion360-Postprocessor how to install at docs.openbuilds.com Easy enough to do. Glue a plastic block in the basin whose top is always above the water level. with the system dry, probe the bottom of the fixture in OBControl, hover over the Z display and write down the absolute co-ordinate. probe the top of the block hover Z and write down the absolute co-ordinate. subtract one for from the other and you now have an offset (height of the plastic block) that you can use in a custom probe macro as though your probe block was thicker by this offset, yet without affecting your normal probing. This custom macro can even go to the block using G53,or you can store the probe position using G30 and use that in the macro. This means you can set your work offset in Fusion to be the bottom of the material = the fixture surface, and tools probed at the top of the block will be at Z=0 on the fixture surface (under water). If you want Z0 to be the top of the stock, then probing 'block + stock + XYZprobe' will give you that, without changing the offset in the macro. A scrap piece of stock from a previous cut should be close enough if you build a bit of leeway into the fusion stock definition.
sommat like that, yeah, having the block+probe offset in the probe macro means that a plain probe on the top of the block is the same as probing the bottom of the material, and probing with a piece of material between the block and the probe is the same as probing the top of the material on the fixture bed.
Right, then yeah, (block + probe) for bed, ((block - material) + probe) for material surface. Adding all of them together would put Z0 under the bed by the thickness of the material. Of course you could use the same thing for both with the macro, just (block + probe), and then have another macro for either G10 L2 P0 Z(current_value + material_thickness) or G43.1 Z(material_thickness) for when you're using the top surface. Depending on whether you want to change the tool length or the coords. Shouldn't matter too much for grbl, would mess up a tool table. Edit: still trying to determine in my head if I've got the signs right in the second part. Would just need to test at a control.
oh Rob, here I am trying NOT to do any math at all (-: so with water covering the material but NOT the red setting block... here we know the sizes because I drew it, but in reality the tool setter block has to be measured as previously described, and the XYZ probe is not exactly 10mm either, but for our purposes here round numbers will do fine. So, probing the tool setter block the macro has to use 19+10 as the Z offset in order for the tip of the tool to be Z0 at the surface of the brown fixture surface. So the macro might be: Code: G17 G21 ; always set expected modes G30 ; go to probe position, previously set with G30.1 as Zmax and XY over the tool setter G91 ; relative move for probe G38.2 Z-90 F100 ; probe down till contact, relative movement with G91, adjust distance to suite your machine (1) G90 ; back to absolute mode G10 L20 Z29 ; make the current tool tip position be 29mm above the 'fixture surface'. your numbers will vary. G53 G0 Z-2 ; raise Z to safety height In effect this makes for a 'thick' probe block, we are increasing it by the thickness of the tool setter to keep the probe block out of the water. And the thickness is simple addition, add the thickness of the tool setter and the probe block together. Now the tool tip Z0 is at the bottom of the material. By allowing for material thickness variations in Fusion360, setting the stock to the max expected (measured!) thickness, the Gcode will work safely across variations of material thickness, but may waste time doing an air cut on thinner material. To set Z0 to the top of the material, we place a piece of material on top of the tool setter (red) block, then the probe block on top of that, and then use THE SAME MACRO to set the tool tip to be Z0 at the top of the stock, in this case 3.1mm above the fixture surface. We don't need to know the thickness of the material nor the signs of the numbers (-: Yes, I know that some machines may run out of Z in this scenario, but if you are cutting sheet you should not be using a tool that is longer than 2x sheet thickness anyway. I have a 3 flute bit I use for carving foam that is nearly 2 inches long and it certainly can suck up Z travel in a hurry since my machine only has 90mm Z space anyway. (1) probe distance adjustment. This should be equal to the distance between the top of the tool setter and the face of the collet nut when at Zmax. This makes sure that even without a tool mounted the collet nut will always contact the probe block on the toolsetter without error.
LMAO. Fair enough. Ooh, the material subtracts itself simply by existing where it shouldn't. Yep, I like that way better!
