Learn FreeCAD: #12 Facing and Drilling - Tutorial

hey guys it's Christopher and in this free cat tutorial I'm going to show you how to generate toolpaths for facing and drilling operations in the paths workbench before I begin I'm just going to show you my tool list I have a quarter inch carbide end mill but I'll be using four facing then a center drill for locating and 3/16 a half inch drill for my drills which will drill these holes these holes are three sixteenths these are 1/2 inch and the 3/16 holes are through holes and these are half-inch deep the depth is measured from the top of my part to the the bottom of the full diameter not to the drill point which is important later so 1/2 inch depth on the half-inch diameter and three one two three sixteenths the block size is just one inch thick by two inches wide and three inches long but that's less important since mostly we'll be working on the face here anyway to get started I will create my job only have one body and I don't have a template for my setup I'll use a create box and add 1/8 of an inch to the top of my stalk the reason for that is so that I can face it off in an operation and I already have the origin where I want it so I can move on to the tools I will go ahead and add all four of the tools that I'll be using and remove the default which I won't need and enter all the data in for my feeds and speeds okay with these values entered I can finish the job and now you're ready to start doing operations before I do anything else I'm going to face it that's this operation right here I'll be using tool 1 my end mill ideally you would normally use a face mill for that but you can use it use a smaller animal too but it shows the path that it takes on the facing operation and I think it it's easier to see with a smaller end know what it's trying to do so that's why I chose that the base geometry going to select the top of my part add that to my geometry and go to the depths so I'm going to start actually 0.225 above my part that's because there's 0.125 on top has stock and I want to leave a hundred thousandths there clearance the final depth is going to be 0 because 0 is the top of my part and the finish depth is going to be 10,000 so that would be the last pass that it takes it's going to be ten thousandths finishing pass and step down I'll leave it a quarter-inch it can take the whole thing as a roughing master then take ten thousandths for finishing Heights they're both above top my stock that's okay and operation there's a couple options here most the time these will go as default one thing I really normally change to be the pattern style if I apply right now you can see the way that it does this facing but I prefer the zigzagged offset that it's the same as the zigzag except it goes around the perimeter to make it covers the area nicely and efficiently there's all kinds of ones that you can try for different styles but I normally use the zig zag offset and the other settings I will keep constant so finish that and now we are ready to move on to drilling this is the drilling operation we're actually going to do this three times because we have to locate all the holes and then drill all of this one diameter and then all of the next diameter so like drill to the center drill if we go to base geometry we don't want to do this feature so we're going to have to go in and select all of these holes make sure we click control as we're selecting and add these to our geometry list there's everything and we can next go to thee we could use a base location actually Sevilla if you didn't have a hole here you can actually just type out the XY coordinate for each one but we have them in our part the depths for all of these I'm going to start actually I'm going to leave it at an eighth of an inch above the part of it then end it negative 1/8 of an inch sometimes you have to add units here or else it'll default a metric for some reason and that should face or not face its drill an eighth of an inch into our part for the four locations these are both above my part so I'll leave them and we won't worry about a pick or a dwell for this and the tip length is not important yet it's just center drilling but those will come into play later so I'll apply okay and you can see that it is drilling down below the surface actually at this point I'm going to animate it show you what it looks like now the reason why it's gonna leave some corners when it's facing the reason for that is because it thinks that it doesn't want to cross the line so far I haven't really seen any problems that it's causing you could just after you're finished you could just file these off but if you're doing high production you would want to find a better solution for that to get rid of corners anyway it looks get center drilled everything properly the depths look fine so we can go ahead and use our drill bits to drill all of these that model there and go on to our next drilling operation which is going to be the 3/16 inch drill based geometry it actually still has it all selected for us and it has the diameters and metric I don't know why it seems like a lot of the things on the path workbench it defaults to metric even if you tell it default to American so I'm just going to uncheck all of these 12.7 this is the equivalent of a half inch hole so I'm just going to uncheck those go to the depths start depth looks okay and the final depth and discard this and make it negative one point one reason is because the block is one inch deep and I actually want it to drill all the way through and take out a hundred thousandths just to make sure I break through the bottom of my part Heights both above the top of my part I'll leave that and the operation this time we will be using a peck what the peck means is that when it goes into your part it will drill the peck length which actually I'm going to set this to one eight seven five normally you use the same peg length that's the diameter of your drill so we have our drill it'll come down 0.1875 come back up and they go down to the place where it left off and go down another point wait so if I've come back up and then go down another one point eight seven five we're sorry 0.1875 it'll do up keep coming down and up until it's all the way through your park the reason is that the reason for that is mostly for chip clearance so that it can clear the chips out of the way before it starts to drill again anyway that's the purpose of Peck drilling I'm gonna keep the peg length the same as the diameter and these are not coming into play yet so I will apply and except now we should have these holes drilled and the last operation actually if we open this up here we can see we have three so far no the fourth and the last operation is going to be done with our half inch drill and most of this is going to be the same actually did not keep the bass drum history this time but we can select all of these half inch holes oops okay and add those to take off the face house here so we just have these four holes depths I'm going to discard this and make the depth negatives your point five because that's the depth of our half inch holes Heights are okay and now we're you're going to get into the dwell and the tip length we won't be packing on this because actually since the diameter is equal to the to the depth it would've only be one pick anyway so it doesn't matter we are going to dwell what this means is when it gets to the bottom of the hole it's going to just sit there and wait while the drill is spinning the reason for this is because if it's spinning and it comes down and hits the bottom of the hole and instantly starts to come back up the hole won't actually be flat because it needs to go at least one full rotation at the bottom in order for it to clear that path actually I like to go one and a half rotations just to make sure and you don't want to go more than that because if it's just down there spinning then you'll rub the financials rub at the bottom of your the bottom of the hole and sometimes it can create a surface finish that's worse so I'd like to go down and dwell for one and a half rotations and then come back up to calculate the time for that you need the RPM we are starting at 600 rpm for this drill which is the same thing as ten rotations per second you take the reciprocal of that it would be 0.1 seconds per rotation which means in one rotation that will take 0.1 seconds and if we want to go 1.5 rotations we would multiply that by 1.5 so zero point one times one point five equals 0.15 and that would be in seconds so we're going to drill down half an inch and then wait 0.15 seconds just enough time for it to spin one and a half times and then come back up it's a little bit complicated and the animation actually won't really show it but that is how the dwell works and we're going to also use the tip length the reason for that is because if we if we did not use a tip length then the tip of the drill would go down half of an inch but we want the tip to go down farther so that the for the first full diameter goes down half of an inch in and that's what the tip length is used for us it's a compensation for that anyway there's a lot of information there and I'm going to apply it okay you can see that the toolpath comes all the way down to the tip where we want it so the tip of the drill goes to the tip of the hole anyway that should be all of our operations if I go ahead and simulate this actually going to turn down the accuracy it just goes faster like this doesn't bug down a computer as much I will run and I get finished and you can tell actually if I hit okay and hide our original body it's pretty pixely but you can tell that it is leaving room for the drill points these are going all the way through and our face looks pretty good except these corners which I not only show how to get rid of on the tool path anyway I think that turned out well we also if you notice in the in a simulation I did take ten thousands Finnish pass on the face which is good so everything looks fine actually you can I don't believe this you can inspect the g-code on itself raishin there we go and you can see everything that's doing first here it's going to do all the facing if I scroll down until I see a G 80 g 81 right here what that means is a spa drilling cycle so that's going to go down and do all of the center drills and if you scroll down a little bit more it cancels that cycle some Rapids and then a G 83 this is where it has the Peck drill this Q value is the Peck amount the Peck length that we set and it's in metric actually all of this is in metric I don't know why it always goes to back to metric but that's the pen Clank and then the X&Y here are the position of the whole scroll down more the g80 cancels that cycle and we get a bunch of G 82's g82 is going to be well the p-value is the dwell value so this is the drilling cycle with a dwell so if you wanted to go back and manually edit this code you actually could after you export it but the peas or the dwells the Q's or the peg length and there's a lot of other letters that mean different things in the g code but those are the main ones for drilling so I think it looks good put my shape back on here and that is a lot about facing and drilling on a CNC anyway I hope this video is useful if it was don't forget to Like and subscribe thanks for watching

Channel: Invent Box Tutorials

Views: 25,609

Keywords: FreeCAD, engineering, tutorial, model, drafting, version, 0.17, path, profile, sketch, tool, beginner, learn, 2019, toolpath, contour, offest, setup, sheet, controller, g-code, gcode, g code, CNC, cnc, milling, mill, tooling, cut, cutting, router, endmill, body, m code, inventbox, invent, CAD, hole, drill, peck, dwell, point, thru, through, depth, rpm, feed, speed, spot, spotdrill, center, centerdrill, locate, location, facing, zigzag, how to

Id: 3vjLlegIm9w

Length: 16min 11sec (971 seconds)

Published: Mon Jan 21 2019