CNC Setup Without Probes—Here’s How! | The Process Ep.1

I'm going to guide you through my machine setup process. We got three ops programmed ready to go into the machine. This is where I touch off all my tools. I got the taper in here that matches a cat 40 holder. I got a cheat sheet here so this tells me exactly where each of my vices are. I'll show you putting a part in the vice how quick it can be without using a probe. Hey everyone, you might know me from the Impractical Machinists podcast. If you haven't checked it out yet, head over to Impractical Machinists YouTube page, click on the podcast section, and give it a listen. I'm Bradley Thomas from Marvel Machining with Impractical Machinists. In today's episode of the process, I'm going to guide you through my machine setup process. This includes programming, setting work offsets, and using an affordable height stand outside of the machine to get my tool length offsets. Rather than using tool setters or probes, I've stepped away from the method I learned many years ago where each tool was manually loaded in the spindle and touched off on a reference point. The process I came up with was just more efficient for me at the time and it's something that I've adapted over the years and it works for me. It works for my machines being I don't have tool touch off in my machines or probes. So let's get started going over the computer and programming and selecting my work system locations on a part. All right, here's the part we're going to program today. Pretty simple part. Go into the feature tree here. Got a couple quarter 20 tapped holes, pocket. So the first thing we're going to do is we're going to come into our stock manager. I already know my stock size here. I know it's 6061, so we'll leave that there. We'll go in, we'll give it its stock size, inch and a half, 3.187, 4.187. And what this is going to do, it's going to center my part in my stock in X, Y, and Z. I'm going to offset my stock from the top in my Z and leave 15 thou just to face that top off. From here, we're going to insert our first mill part setup. I'm going to go from this top side here and in my mill part setup, I got face option perimeter. So we're going to go open pocket. So this will rough and finish it and then curve feature for chamfer. And this is going to recognize any edges that it can chamfer. This is just a quick setup here that gives me a couple features and strategies that it's going to automatically recognize the stock and put it on its own. So what that does, it puts in my face feature, part perimeter, open pocket, rough and finish, and then the edges that can chamfer from that top view. We got to add the pocket and the two threaded holes. So from here, we're going to right click, go into mill part setup and recognize the features. This should pull out the additional features. So now we got a rectangular pocket, rough and finish, and then our two threaded holes here. I'm going to generate our operation plan, go into our mill part setup so we can tell it where our origin is going to be. I'm going to select my stock vertex. I'm going to give it this bottom left corner. X is facing the wrong way right now. So we're going to flip that 180, give it its work coordinate G54 here, hit okay. Now from here, we got all of our operations. We can go in here and change all of our parameters. I'm going to let it, it knows my stock is 6061. This knows all my parameters for 6061, my feeds and speeds, so I don't need to change anything. The only thing I need to do is I need to move this tool 24 quarter countersink tool down and then generate my tool pass. So we got a face, face mill operation, outside profile, rough mill, contour mill to finish the outside. We got a pocket operation, finish, center drill, drill, chamfer the edges, chamfer the threaded hole, and then tap it. Do a quick simulation for this first stop. So here we got the first stop program. Checking for any thing crashes. If anything's red, we're good to go there. So now we're going to go to our second op. I'm going to flip it over, insert mill part setup, top feature here. We're going to face it. We don't need a perimeter on this one and we'll leave the curve feature for chamfering so I can select that top edge. Face feature, edge break, generate that operation plan. Now this is our second op. We're going to select this bottom left corner for our work corner offset. We're going to go to G55 here. Okay, generate tool path. Again, my default values are already in here for my parameters for running 6061. Now we can simulate the second op. Face, chamfer the edge, second op is done. We got one more op on the top here. So we'll go through the same process again. Mill part setup, top feature, no face, no perimeter, no curve feature. Okay, we're going to recognize the feature so this will pull out that threaded hole. We don't need a face feature. We don't need any of these. Generate the threaded hole operation. We got a center drill, drill, chamfer, and tap. We'll go into our mill part setup here. Give it our work coordinate offset. We're going to go to this bottom left corner here, the theoretical corner. We'll leave this offset 55 because I'll use the same vise with some jaws and parallels here. Generate tool path. Now we got center drill, drill, countersink, tap. So from here we can simulate the whole part. Make sure there's no shank rub, tool holders hitting anything, and all the stock is removed. And then we got three ops programmed ready to go into the machine. Tool crib, so it added my drill, my tap. These three tools here are already loaded in all three of my machines so I know they're in there with your height offsets. So we're going to add tool one and tool two to the machine. So now that we got that, we're going to go over, load some tools into some holders, and then I'll show you how I touch my tools off and get my values with my height stand. This is where I touch off all my tools. The system I got here, this tool block, I got the taper in here that matches a cat 40 holder. And this setup works across all three of my machines, my vf2, my vf3, and my horizontal. If I take my 3d sensor here, dial this down, bring the dial around to zero, this value here is minus 13732. So what I'm going to do is take this over to my machine and put that value in my height offset for this tool. We're at the machine now. We're at a tool offset. I'm just going to use tool one for an example. So the value we got from the height stand, I'm going to put in here minus 13732. Now we got that in there. We're going to load this 3d sensor into tool one, and then I'll show you where that number correlates to the work offset, which we'll go in here and we'll just set our g54 at z0. And I can show you where this number and this number line up. All right, now that we got our tool loaded in in tool one, we got our offset in there and our g54z set at z0. I'm just going to manually feed over above my vice bed right here and show you where that z0 comes in with the tool offset length. All right, I have my 3d sensor in here. I have it positioned right above my vice bed here. So we're going to go into MDI just to give a demonstration where this is going to end up when I bring my tool one to z0 off my g54z0 work offset. So if I go g90, g54, end of block, g43, h1, z0, end of block, m00, end of block, enter. I just put the m0 there just so it doesn't go into my preset MDI data that I use. Set the rapid at five percent and we'll hit cycle start and this should go down and zero out on the top of my vice bed. There you go. Now I've demonstrated how touching a tool off with the height stand outside of the machine, taking that value, putting in a tool offset, and where that correlates to my machine's z height offsets in the work coordinate system. My vice bed, as I said, is z0. From there, when I put parts in my machine, I always know where my z is. I showed earlier programming that I program from the bottom of my stock on my first op. Any additional ops that I flip over, my z work coordinate system is from the bottom of that finished surface. That allows me to always know where my parts are in the z. It doesn't matter if I set them on an inch and a half parallel. If that part's sitting there, my z value in my work offset is going to be inch and a half. So the next step from there is knowing where my x and y is. I got a cheat sheet here. So this tells me exactly where each of my vices are. The center locations. I know the width of my vice. I know where my y is at on my vice with the jaws in there. And I got a quick reference here showing the height of everything and a couple quick features here. My Heimer height, my curt jaw face, where everything is. So most of the time when I stick a part in my vice, I know where it's going to be in the machine based off these values and building my fixture plate here and doweling devices in location. So I know where everything is. It makes setting up a little bit more efficient in most cases. From here I'll show you putting a part in the vice, machining a part, using these values here, how quick it can be without using a probe. For my first stop, I'm going to set the part here and use the seri grippers to grip on my first stop on the stock here. Now I know the vice bed is z zero. So if I take a quick measurement here, my z is 1.688. That's where my stock is going to sit for that first stop. I'm going to put that in there. And now to establish my x location, I'm just going to use a gauge block here and I'm going to line it up with the left side of my vice. With my stock and the vice positioned where I need it to be, my cheat sheet here, I can put in my g54 values. Now I know that center of that vice is at minus 24.6. So we're going to put that in. Now I set my stock to the left side of that vice. I know my vice is six inches wide, so I can adjust it another three inches making it 27.6. Now my y, I know my seri grippers y location is at minus 4.934. So I'm going to put that in there and then my z as I showed with the calipers at 1.688. So now I got my g54 x, y, and z location figured out and set without using an edge finder, a 3D sensor, a probe. These are just predetermined values based on my fixture plate and my vice locations. So now we're going to touch off the rest of our tools and get them loaded in. Tools are in. Offsets are in. Now we got to load our program and hit cycle start. First op's done. Now we're going to flip the part into the next vice for a second op using g55. I'm going to use some inch and a quarter parallels to set it on. We're going to flip it over and I'm going to shift the part over to the left side of the vice and touch it off the gauge block, line it up, clamp it in there, tap it down on the parallels. Now I know where my g55 is based off putting the part in the vice and located it off the left side and I already know where my y is and my z is going to be inch and a quarter because I'm using inch and quarter parallels and I programmed from the bottom of the part up. Now we're ready to run the second op. That's my process on how I set up my machines from selecting my work quarters system when I'm programming my work offsets in the machine to setting tools outside of the machine using the height stand. Now if you got a probe or a tool setter in your machine, probably irrelevant but a lot of us don't. A lot of us are still doing it the old school way, putting tool in the spindle, hand feeding down and touching up on a reference point. This is just another option if you're looking for a little bit more official way to set your tools or your work offsets. Another tip is if you use tool tags, I put these on all my standard tools. I leave my height offsets on here so I can just grab it from the car floor to the machine and it's ready to go. And these tool offsets, like I said, they're universal from my horizontal to my bf3 to my bf2. That's how I set up my height stand so it all just kind of drives together. It makes it a little bit quick for me to set up any of my machines or pull a tool from one machine, put it in the axe and not have to pick it up again. So that's my process. If you'd like to see more, comment below, let me know, click like, subscribe, and stay tuned for more from the process. Thanks for watching!