Fusion 360 DXF Import Tutorial MillRight CNC

so we had a customer ask us how to do a DXF import with fusion 360 let me take you guys into fusion 360 and show you how that's done all right here I am with a new design I'm starting blank you should have an insert option then you'll go to insert DXF need to select the plane that you'll put the sketch on see I rotate my cube around I have three different planes to choose from for simplicity I like to choose the plane where the z-axis points up that'll help me a little bit later when I'm moving to my cam settings alright I selected that plane now I'm going to click the folder to select the DXF file here I have a sign that I designed quite a while back using Inkscape I saved it as a DXF file from Inkscape and now i'll import it here you should know that you can also import an SVG file so if you just start with an SVG file you can work directly with that infusion I'll click open and fusion will bring it in you notice depending on how it was designed it may not come into your workspace the way you'd like in terms of where it is in respect to the origin but we can deal with that and can I'm just going to click OK here now the first thing that I want you guys to realize is that not every DXF file are actually very few DXF or SVG files we're going to come in the size that you want to make them so we need to take a couple of measurements here see how large it actually is and get it where we want it so here's the formula that's going to help you understand how to scale the sketch that you've been ported that sketch to being that DXF file that we just imported here's how you're going to scale it you're going to decide what your desired length is for a given dimension and then what the actual size is of the imported file and that's going to give you a scale factor so let's say that I want across this sign I want from here to here to be 400 millimeters that's about 16 inches and that'll be good for the mill right CNC carve cane now I'm just going to measure it if you didn't see what I did there I just went to the inspect tool and I'm gonna click these extreme points here here to here I got 14 28 point seven five one now I doubt that I originally designed it to be 14:28 point seven five one millimeters from there to there but a lot of times when you're moving from one program to another things get a little distorted in your files so I'm going to take that measurement 1428 point seven five one I'm just going to type it there okay my desired size is 400 millimeters so I want that size or that length to actually be 400 millimeters from here to here I measured fourteen twenty eight point seven five one using my inspector measuring from point to point what I'll do now is I'm just going to divide 400 which is my desired size divided by my actual size of 14 28 28 roughly I'm going to get a scale factor of 0.2 eight so here's what I'll do with that scale factor I'm going to go to modify and I'll select the drop down here scale the entity that I need to select is this sketch the scale factor needs to be 0.28 and you see it's scaling it here and showing you how large is going to be relative to the model that you started with now I'm going to click OK alright and it's going to give me some warning here that it failed to compute I doubt it I think fusions just freaking out a little bit it seems like they computed properly okay zoom in here let's say I want to make something out of this file now alright here I have a family sign and what I've done with this before is I've pocketed these letters down so it's recessed into the stock and it makes for a nice look so let's say I'm starting with some 13 millimeter MDF I'm going to left-click on this face I'll right-click then and tell it to extrude I'll extrude it to 13 millimeters now you don't have to do this here but I'm going to do it because I think it'll be easier when we move into our camp settings where we set up our tool path I'm going to click each one of these features and I'm just holding the ctrl button as I click to make sure I select all of them at the same time let's say I want to pocket this down three millimeters into the stock so let's think about this a little bit I just extruded this to 13 millimeters so this space here that I'm highlighting now with my mouse is 13 millimeters high okay if I'm starting from the same plane I need to extrude this up 10 millimeters if I want them to be 3 millimeters recessed from this space don't let that confuse you just 13 minus 10 is 3 and you'll see what I mean when I do it I'm going to right click and extrude going to extrude to a distance of 10 millimeters okay now one thing that I should not have done there was let it's a new body and we're just going to show you that again repeat extrude I should have told it to join but it looks like fusion 360 took care of me anyway sometimes if you don't specify that you want it to join to this existing body then it's going to create several new bodies in your tree here if you have body one body two buddy three but fusion 360 took care of me it knew what I wanted to do here alright so I'm gonna go ahead and turn my sketches off and you can rotate that around and you see what I'm talking about here if I take my inspect tool and I measure from here to here the distance is three millimeters which is what I wanted so now let's move over to the cam side now that I've got the model the way I want it you'll notice before I go to the cam side I like to turn the sketches off even though the bulb was still on for the sketch I've turned all sketches off by this bulb being under lit I'm going to click on cam and I'll do a setup every cam operation starts with a setup okay you remember from our other video you need to go to stock and tell her that you do not want to add any additional stock sometimes you do in this case we don't okay I'll go back to setup and it's trying to set the origin in the middle of the park that works for me in most cases this time I actually want to put it here because when I go out to the car of King and I set this up I know that I've got only so far of X travel to deal with if I just start over there close to the left side close to the negative x direction and give enough room for my tool path for my outside contour I know that I'm safe when it just travels 400 millimeters here that way I don't have to do a lot of figuring to make sure I'm going to be within and below this won't always be the case so you need to be strategic when you set these orientation points this works for me for this model so I'm going to move forward by clicking okay all right the first operation I'd like to do here is a pocket operation right I'm going to go to 2d 2d pocket the tool that I want for this is going to be a one-eighth inch end mill and three point 175 millimeter is one-eighth inch I'll select that this is something I set up previously just so I could have a two flute now the flute count will impact or feed per tooth this will automatically calculate based on the number of flutes in your tool and the feed rate and spindle speed I'm going to turn coolin off because there's no need for it and the machine's not even equipped for the coolant system if you left it on it would be okay it would just kind of clutter the code with extra M codes I'll disable that you can remember from a previous video our spindle speed does not matter if you're running one of the mill write machines it doesn't matter because most likely you have not set it up for pollenated spindle controller or spindle speed control you're manually turning a knob or setting the speed on your router where it does matter is calculating your chip load which is what fusion 360 calls feet per tooth you can find different chip load charts on the internet for the material that you're working with and the different tools that you're using so the recommended chip load for say a half-match cutter is going to be vastly different than the recommended chip load for a 1/8 inch cutter you also might want to consider D rating some of the chip loads that are recommended they're often intended for industrial machines that can handle large cutting forces that a hobby level machine like the mill write or many of our competitors won't be able to handle so I'm going to be using the DeWalt d WP 611 I think I want to run this at about 24,000 rpm I'm gonna have a cutting feed rate of about say 1500 millimeters per minute that's going to give me a chip load that I'm pretty satisfied with I'll leave in because it's a soft material I'm going to lead in very close to my cutting speed rate I'm also going to ramp at about the same speed that I'll lead in and lead out with my plunge rate I'll just set the 300 millimeters per minute now I need to select the geometry I'm just going to go in here because these are the areas that I want the Machine I want to show you something here fusion sometimes does something kind of odd I'm going to close these selections notice when I select this one it just seems to highlight within the feature that's okay this one here it wants to blow it out in most cases it's going to machine fun anyway but just be careful how it generates the toolpath when you see this happen we're just going to go on and select the bottom of each pocket okay the heights I encourage you to leave alone until you understand all of the different options it's kind of complicated and that you're setting these heights relative to different points in the model so fusion 360 will most likely take care of you if you just leave it as a default your passes is important notice that it wants to leave stock that would be if you were coming on with another operation you wanted to perform say a finishing clean up on the inner contour here I'm going to turn that off by default fusion 360 wants to machine all the way to the bottom depth of the feature that you've designated to machine I'm only doing three millimeters deep here with an eighth inch end mill so I'm just going to let it do that in most cases however I've set the multiple depths and then decide how far it can go with each step down I'm not going to do that in this case on these particular features I'll move on to my linking tab here it's going to by default helix and to the stock and this is only with a pocket operation and some other operations in Fusion if we were doing a contour operation by default it's just going to plunge into the stock which is not ideal for an endo I'm just going to accept the default settings for the ramp and click OK it's going to take a little while to calculate the pocket operation because it's a little more complex so we'll just be patient and we'll see how it comes out we look through remember how it made that big blue circle that seems to be a glitch but it looks to be machining properly one thing you want to watch out for on small features is that the cutter is going to actually be able to get in there and machine it I intentionally chose a small end mill to 1/8 and built to make sure that it got into all the features as I look through I'm pretty satisfied with that tool path I'd like I could simulate that but I'll do that later let's move along now to a contour operations that we can cut this out I'm actually going to choose instead of the 1/8 inch end mill on this one I'm going to do a quarter inch end mill you don't always need to change to a different tool what's going to drive that is the chip load that you desire so that's also going to be determined by how fast you want to feed what your spindle speed is and what your machine can handle I'm going to go with the six point three five millimeter also quarter inch that I've set up before and I'm going to machine this contour so what I'm doing is I'm going to let this quarter inch and they'll run around and cut this out okay I'm going to change the settings that I had set up for this tool go to 2000 we'll leave this at a twenty four thousand that we had for the other operation will lead in at eighteen will aid in an eighteen or laid out at eighteen will ramp at eighteen hundred and will plunge it three hundred for the car came this is a pretty conservative setting I'm going to leave tabs on this particular one because I don't want it to move as I machined by default fusion 360s but far more tabs and I need to hold this in place so I'm going to make some adjustments here so I'll have quite so much work to do once it finishes I'm going to change the tab distance to 150 we'll take a look at what that does now I have a tab here and a tab here it's like I've got another tab there in there and that should be sufficient for holding the piece down as it's cut out again the heist tab we're going to label all fusion 360 does a good job of designating this for us based on the contour that we've selected in the Passons tab we definitely want to make sure we select multiple dips we don't want to machine all the way down in this 13 millimeter piece of MDF the carpeting is not going to do it nor are any of the competing machines machine all the way down 13 millimeters at one time let's go ahead and make that four millimeters that should be a good setting for the carve king and still pretty conservative I want to use even step downs and what that's going to do I've designated four millimeters here so it's going to go four millimeters deep eight millimeters deep 12 millimeters D then would have one more path to go if I did not select use even step downs the point is that with a four millimeter maximum step down that 13 millimeter model it's going to have to make at least four step downs what they use even step downs is going to do is say well let me just divide the step down distance by four then click OK and see what we get as you can see it's used even step downs if I didn't do that then it would come for D another for D another for deep and it would have just this one millimeter left sometimes that's useful sometimes it's not as I look over my tool path I realize that I've forgotten to do something that I normally do here we see the tool leading into the stock which is desirable because that will minimize the artifacts of the cutter left on the finished piece if you don't do that a lot of times you actually see an end mil mark say right here where it comes in you're not going to necessarily get all the way away from that but the lead ends in lead else will help what I'm talking about though is I did not set up any kind of ramping entry into the stock it's trying to plunge directly down to each death as I said before that's not ideal for an input I mean it right-click tell it to edit I'll go to linking I'm going to click for it to ramp will just accept the default ramping settings for now we could definitely more aggressively but we won't get into that for now click ok and you see here how it's now ramping into the stock versus plunging directly alright now we can look at our tool path together and make sure that we've machined everything we want to I think that looks pretty good let's simulate it just to be sure you'll notice that when you're trying to do the simulation you've got this big tool holder in the way it's not actually going to be on the machine so we can just change it just a flute and we'll see just the cutting fleet doing the work there if you'd like to see the stock removed as it simulates you can click stock and you'll see what it's actually going to cut out and this is a good way of seeing where your cutter won't actually get into and what stock may be left over that you don't expect to be left well fast forward all the way through this so we can see to the end of the simulation ok looking through it I'm pretty happy with the simulation so we'll move forward now if you remember the pocket operation we're using a 1/8 inch end mill and the contour operation we switched over to a quarter inch I do not want to try and run those at the same time if I do that at the same time it could just move on to the next operation if there's no Paul's command placed into the g-code file so I'm going to actually post-process these separately I'll run the pocket operation with a 1/8 inch end mill that operation will finish then I'll change my total L to a quarter inch in and I'll run the contour operation so I'm going to select just the pocket op we'll go to actions and then post-process you need to make sure that you are on verbal dot CPS that other machines that run Mach 3 so we need to move back to Google if you don't do that you may end up with some odd behavior or some skipped commands I like to turn g28 off I won't get into why but just take my word for it for now I like to leave open and open NC and editor checked so I can make an edit to the g-code I'm going to name this something relevant all that family pocket now I'm going to click post I'll just save it and the file that or the folder that opens by default you want to make sure you put it somewhere that you can find it though click Save when I click Save my editor is going to come up the program called brackets if you've never done this before then fusion 360 is going to try and download bracket I want to get rid of g54 this is a work coordinate selection command I like to leave this out of my G code because I not always end the g54 system maybe I maybe I'm trying to make 50 of these signs and I've set up a clamping jig and I've specified the origin as the origin of the g55 system if I run this it's going to try and switch coordinate systems over to G 54 now at fusion 360 allows you and your cam set up to change the coordinate system you could change that to Chi 55 or G 56 or whatever you'd like I like to avoid the issue altogether and select my coordinate system when I'm actually setting my machine up to run the file I'm going to delete that and I'll change it to G 0 Z 10 now what this is going to do is make sure that my cutter is lifted up above the stock before I actually begin to reversing in the XY plane if I wasn't paying attention to what I did and let's say I just zeroed my cutter to the stock and then trying to run this it might skim that cutter all the way across the stock and potentially ruin my piece if anything was not perfectly level so I'm going to get rid of the g54 I'm just gonna put a Z lift and I'm gonna go to file/save we can move now to our next operation I'm going to select contour and I'll go to post process again here I'm going to say family side on tour I want to make sure that g28 is still off and I'm open again see file and editor I'll save that and I'm going to do the same thing here but I get rid of my G 54 change to G 0 Z 10 I'll save the file now that's a wrap on how to import a DXF file turn it into a 3d model and set up camp and generate G code if you've got any questions let me know I'll see how I can help Thanks

Channel: MillRight CNC

Views: 34,360

Keywords: millright cnc, millright, fusion 360, autodesk fusion 360, fusion 360 dxf, fusion 360 cad, fusion 360 cad cam, fusion 360 tutorial, fusion tutorial, cnc machines, cnc router, cnc cad cam, shapeoko, x carve, 3020 cnc, 6040 cnc, bob's e3

Id: I1JMBFXyyVU

Length: 23min 30sec (1410 seconds)

Published: Wed Aug 30 2017