Making a Torch Splash Guard | Langmuir Crossfire Software Workflow | Fusion 360 Sheet Metal

today we're going to make a sheet metal part with the new cnc plasma table and we're going to walk through the entire workflow from the cad to the cam to cutting it out to folding it to shape stick around welcome back to cloud42 i'm james well if you've been around the channel long you have seen my cnc plasma table and you've seen my new electromagnetic sheet metal break and today we're going to use those tools and actually make a sheet metal part now i've gotten a bunch of requests to talk about the software workflow for the langmuir systems crossfire plasma table and to be honest the documentation that they provide on their website is not great if you have just the basic table then they have a series of videos that walk through all the steps but if you have any of the optional accessories like the z-axis or the torch height control then you have to ignore certain parts of the video and supplement with written documentation on the website and you have to figure out how to put it all together now i've done that and i've got this working and i've got the workflow sorted out and we're going to walk through that today and that process starts with designing the part that we want to make the first part i'm going to make on the plasma table is not a surprise if you know me very well it's an upgrade for the plasma table and if you go out and look at the langmuir forums there's lots of references and lots of people have models for these torch shields and the idea is the the plasma torch is going to splash up water from the table and it's going to get onto the handle and in particular into the trigger switch and so there are several designs out there for these sheet metal shields that just go on the two screws of the clamp to shield the torch from that water splash now i started out by just trying to come in here and download one of these and i didn't get very far the one that i picked had a bad dxf file at least it didn't import properly into my tools so let's just skip all that and design one ourselves so this is one that i designed in fusion 360. of course you could use you know any cad program to do this but langmuir systems provides a cam post processor for fusion 360. so that's what we're going to use and it wouldn't be any fun to just use one that i prepared earlier so let's design one from scratch now we're going to design this part in the sheet metal workspace so we'll just come over here and click sheet metal and the first thing we need is a sketch and i'm just going to put this sketch on the x y plane and we will start with a rectangle pull this out set that down i'm going to hit d for dimension and let's give our rectangle some dimensions say six and a quarter inches long and two inches wide now i'm working in inches you don't have to work in inches this works just fine if you have your document set up for metric i have mine set up for inches because that's convenient for me so go ahead and rage down in the comments about how inches are inferior i know that so we'll finish the sketch here and we will create what's called a base flange so whenever you're working with sheet metal the unit of work is the flange so i'll select this area come up here and click flange and i have to select a sheet metal rule that i want to use now we have an aluminum that's aluminum millimeters aluminum inches default and this is not for the thickness of aluminum i'm going to use i'm going to use o50 aluminum 50 thou and again you can do this in metric if you want so i'll just accept the default and then we'll come up here and click modify sheet metal rules and we'll modify this rule for the sheet metal we're going to use click the pencil to edit it and my sheet metal is not 080 it's o 50 and you have the k factor here you can specify which specifies how the material bends 4 50 h32 aluminum 0.44 is a reasonable guess you can calibrate this by actually bending your material but i'm just going to use all the defaults in here because we're not trying to hit an outside dimension on square corners with this i can leave that for later so that gives us our sheet metal rule and then now we can start pulling up the other flanges so i will select this top edge here of the end click flange and i will pull up a flange and i'll bring this up 0.6 inches and now we have actually built a bend and there are a bunch of parameters if i go back in and look at this flange you can control whether the bend position is inside meaning that this outside face will line up with the end of the part that it was pulled off of so you can see that that bend pulls up so that it is inside the part you can set this to outside or you can set it to adjacent so that the bend is all outside the end of the part however you want um i generally use inside unless i have a reason to do otherwise so pull that up 0.6 inches and this is going to be the plate where we're going to screw it in so i'm going to right click here and create a sketch l for line set that to construction and we'll just pull a couple of construction lines across aligned with the midpoints create a point and then mirror that point around this center line then hit d for dimension and i will dimension those two points i know these are 1.55 inches apart because i measured on the plasma table after i already made one 1.5 inches and it didn't fit so that gives me my two points and we can go back over to the solid workspace select hole pick both of those points set my holes to it's a quarter inch screw so i'll make it point to six inches so there'll be a little bit of clearance okay and that gives us our holes through that part go back over to sheet metal and we need the wings that come up on the side so i'll click this top edge here click flange we'll pull that up we want that about an inch and a half but i don't want it at 90 degrees let's pull that out at 55 degrees okay that looks good and then we want one on the other side as well so i will do a i'll select construct here and i will say mid plane and i'll just select a couple of planes that are on opposite sides of our part that'll give us a mid plane that's right down the center and then we will go back to the solid workspace here and select mirror i want us i want to actually mirror a feature and the feature that i want to hit mirror is this uh this flange and the mirror plane will be the center okay and so now we have a flange on each side now we're almost done i want to go ahead and curve some of these corners so hit f for fill it and i will just select some of these corners and let's see 0.5 inches that looks pretty good for that f again we'll fill up these corners 0.2 looks pretty good and then i want to fill up this corner down here too 50 thou looks pretty good now if you take a look at these corners you can see that fusion has automatically added some relief here so that the bins don't collide and crease up in the corner there's a bunch of settings in the sheet metal rule for exactly how that's handled but we're going to ignore that for now let me turn off our construction and this is the part ready to make of course to actually make this part and cut it out it's going to be flat so let's go back to the sheet metal workspace and let's click on create flat pattern so i'll click that they want to know which stasis face is stationary click here click ok and now we have a flat pattern of the part and based on the k factor and the other parameters in the sheet metal rule fusion has automatically added bending allowances here so we don't have to add extra material or think about that ourselves if we cut this out and bend it and if the k factor we provided in the sheet metal rule was correct then the part will come out the right size now i can click up here and just say finish flat pattern to close it and go back to the part and then the flat pattern is over here in the tree and i can activate it any time just by selecting it and now it's active i can actually do work on the flat pattern click finish flat pattern it goes back to the 3d model now to actually cut this part out we need to set up the g-code for it and we do that over in the cam workspace i'm going to first activate the flat pattern because the cutting is all going to happen from the flat pattern so i'll come up here where it says design and pull this down and instead select manufacturer and this will take me over to the manufacturer workspace and we've got the flat pattern open here and we're going to use this to set up our cam first thing we need is a setup so i will click here to create a new setup and i'm going to come over to operation type and set this to cutting by default it's set to milling which is what i often do but we're going to be cutting here and so the first thing i need to do is get the work coordinate system set up and i'm going to click the body of the y-axis here and click a line on the left of the workspace so or then the work piece so it's going to align the y-axis in this direction and click the head to flip it over to the other side so this is the orientation i want now i'll click view origin and click this top lower left corner so now we have our zero point on the top of the sheet metal in the lower left corner with the y oriented the direction that i actually want to cut this then for the model i'm gonna click body here and i'm gonna click on the flat pattern so we're gonna designate that this flat pattern is the model that we want to cut out we're going to go over to stock and define what the material is we're going to cut out of relative size box is fine stock offset mode is set to add stock to sides and top and bottom so on the sides i'm going to add a quarter inch on all sides and then the top and bottom i'm going to add zero so this is as far as it's going to know i'm going to have a piece of sheet metal i'm going to cut this out of that it's a quarter inch larger than the part on all sides in reality it'll be a much larger sheet but that doesn't matter and we can just click ok and now we have our setup so now we need to add a cutting operation so i'll just click up here cutting which is a 2d profile and the first thing i need is a tool and if you don't have anything set up i actually already have some plasma cutting tools defined but we can go ahead and just add one so if you don't already have one you can come in here and just hit plus and choose the kind of tool and we're going to create a plasma cutter tool and we can give this a name standard consumables on the hypertherm and on cutter the most important thing is the kerf width and i know that my plasma cutter is about 50 thousandths curve width with the standard consumables you can oh 55 is kind of pretty standard but you can look this up for your plasma cutter or you can experiment to determine what it is and for the nozzle clearance diameter i'm going to say that my nozzle is about an inch in diameter and it ultimately just uses that if the nozzle is going to stay down and it needs to steer it around existing cutouts in case something tips up because we're going to use the torch height control it really doesn't matter that much you can define holders and and other kinds of cutting data in here but it really doesn't get used because the cutting feed rates are going to be defined in the program and the output for the post processor doesn't really matter because we only have the one tool with the plasma cutter so we can just hit accept and now we have our tool defined and we can just select that and go back to the 2d profile that we're trying to set up now i'm going to set the cutting feed rate here to about 150 inches per minute and i'll just go ahead and set the lead in lead out all these to 150 inches a minute this is dependent on your plasma cutter the current and the type of material and the thickness i know because i've experimented that this material that i'm using this o50 aluminum cuts pretty well with the standard consumables on this 30 amp plasma cutter that i have at about 150 inches a minute and this will definitely vary depending on your tools so then we need to go in and select geometry and we're just going to select the contours that we want to cut out so i'm going to cut out this hole and this hole and the entire outside of the part now these arrows indicate where it's actually going to cut so if i if for example this arrow here is on the inside if i click it'll flip to the outside and it'll actually try to cut around the outside of this i actually do want it to cut around the inside so this one's going to cut around the outside these are going to cut around the inside we can go in and look at the heights the heights don't matter because the torch height control is managed by the um by the post processor the stuff here on the passes does matter we want sideways compensation set to left this is because of the the swirl direction on most plasma cutters compensation is in computer meaning that the computer is going to actually keep the curve on the correct side of the line and then over on linking this is where we need to set our lead in and lead out and sweep angles this has to do with where the pierce will occur and how the cutter moves into the cut and the real issue here is just that the these holes are small if we just take the defaults we'll be fine on the outside but to make sure that we're piercing somewhere in the middle of this hole we need to change a couple of these lead in radius i'm going to set this to .06 inches 60 degrees i'm going to change this to 90 degrees and we need zero lead in distance and then we're going to set the pierce clearance to 75 thou now i played around with these you can play with these to get it where you need it but i've played around with it and this does a pretty good job of getting the pierce to occur inside the center of the hole in a place that's reasonable if you don't um if you don't have this set correctly you might end up trying to pierce some place outside the hole or in this case where we're cutting inside if it knows that the pierce is going to be is going to interfere with the rest of the work it just won't generate a path in here and you have to go back and play with it now i can see i've got a lead out here i don't need that so i'm going to double click on this to open it back up and i am going to uncheck the lead out and that makes sense well pierce will cut around the part and then we'll pierce here and cut around the exterior so let's simulate this come up here and click on simulate and click go and we can see what the plasma cutter is going to do and this looks entirely reasonable now that we have the tool path all planned out we just need to generate the g code so i'll come up here to post process click on this and the first thing we need to do is select a post processor now langmuir systems provides a post processor if you come up here to their website and go to the downloads page under post processors they have versions depending on which version of the table you have they have different post processors and here's the one that i'm going to use which is the fusion 360 post version 1.6 just click here and it will download it i already downloaded it and then you go back into fusion and here where it says post we'll go ahead click the three dots and we will click import and go to the downloads and in select the file that i just downloaded which is this fire control 1.6 cps now i actually already have it in here because i already imported it and when you import it you can import it locally on your machine i went ahead and imported it to the cloud so it'll be available on every system where i start fusion and so i will just click select and it will select that post then i need to select an output folder for where that file is going to go and i will just select a location and then i there's an option down here opennc file in editor i like to do that so that i can see the file that it's generating and then here's where we set up the height information for how the cutter is actually going to behave now with the particular torch that i have in the particular cnc shield that i have i know that i want the cut height to be 35 thou and we're going to count for maybe 10 thou of spring back this is when the torch goes down and probes and finds the work height this is how much we expect the metal is going to spring back when the torch comes off of it so this is just to correct for errors due to the metal flexing when we probe it ihs is the initial height sensor i have that so i'm going to leave that checked pierce delay we're going to go with point six inches and again i just determined this by playing around with this material pierce height uh height is going to be set to 125 thousandths and then retract height is one inch so it's going to cut at a height of 35 thou it's going to pierce from 125 thou and then at the end of the cut it's going to retract up to an inch to clear the work piece and let the and that's for moving around to avoid tip ups as we move the torch to the next cut and we have the box checked for the torch height control because i have that option on this on this plasma table so then we can just click post and it will generate the g-code and it's already generated it and here it is loaded up in visual studio code if you don't have this it'll prompt you to install it or you can just say you don't want to preview it and not even worry about it there's a bunch of mysterious stuff in here and i didn't understand what it all meant so i took the time to look it all up and i have another version of this file that i've already annotated and so let's walk through what kind of g-code it's generating and what it does the first part of the code here is just a preamble to set up the defaults so that the interpreter is ready for the g-code that's coming so g90 puts it in absolute mode meaning all the coordinates will be absolute offset from the zero zero position and g94 tells it that all feeds are going to be per minute so if i say feed 150 it's going to be 150 units per minute g17 selects the xy plane for cutting and g20 sets it to imperial inch coordinates this would be different if you're doing metric h0 turns off the torch height control and that's because we're just trying to zero everything out we are not cutting yet we're just going to switch that off to make sure it's not confused so this gets the plasma table into a known state and the first block here is to cut out the first hole so g0 is a rapid it's going to move rapidly to the x and y coordinates of where it's going to start the first hole g92 resets axes so it's going to reset z to zero so whatever height it happens to be it's going to forget what we what it thought the z coordinate is it's just going to set it to zero then the next two are a two part probe g38.2 is going to probe until the torch height control switch makes contact so z minus five means it's going to go down five inches at a feed rate of 100 inches per minute until it contacts the work piece so it's trying to find the zero height of the of the sheet of metal that's in the table now that's because it's moving pretty rapidly that's not going to be very accurate so then it's going to do a g38.4 which is going to probe until the switch loses contact in an upward direction half an inch at only 20 inches per minute so it's going to go down rapidly until it makes contact then it's going to go up slowly until it loses contact so at that point the torch should be touching the work piece so it resets z to zero again then it moves up thirty thou now this is a combination of the spring back that we uh that we actually put into the post plus the back backlash that they know would be in that z-axis so that they're estimating in the z-axis um just based on the design of the z-axis and so they're moving this up so they've taken out that spring back and backlash and reset z to zero again so at this point this should be an accurate probed height so the torch is sitting right on the surface of the work piece now we're ready to cut so it's going to move up to our pierce height it's going to switch the torch on and it's going to dwell so it's going to pause for 0.6 seconds that's the dwell that that's the pierced time that we put into the post so it's waiting for the plasma jet to cut through the metal then it's going to wrap it down to the cutting height turn on the torch height control so it's going to start monitoring the voltage and maintaining whatever height it's at right now which should be the 35 cut height we programmed and then it's going to start making the move to actually cut out the hole so g1 is a move and then g3 is an arc and it's going to actually cut out the hole then switch off the torch height control switch off the torch and then raise the torch up to the z retract height up to one inch and then it's going to repeat so for the next hole it's going to move to the location it's going to do the whole probing sequence cut it out turn off the torch then for the outside perimeter we'll do the same thing move to the start position probe it pierce go to the height turn the torch height control on cut all the way around the perimeter and then turn off the torch raise the torch to an inch and then that's the end of the program so this stuff's pretty straightforward and it is actually a pretty simple post processor because there's very little it has to do just has to probe set the heights and actually move the torch around to cut so i think that's it for the software let's go out to the plasma table and run the program and cut something out the first step is to load the gcode file that we just made here into fire control and i will just click the upload button and we will choose here it is one zero zero one and c and it will load it into fire control and we can see here it's generating a visualization and this is exactly what we expect so we can see the zero point in the lower left corner and the path up to cut the two circles and then the path around the outside and so now we just need to set the zero point where it's going to run so i'll use page up and page down to move the z axis get it down close here and then just drive this around with the arrow keys and try to get close to where i want to be let me so that's about the lower left corner and there's plenty of material there so we'll reach up here and hit zero all axes and we can do a dry run of the program i'm gonna go ahead and raise the torch up i'm gonna zero this up higher so hit zero all axes again the z height doesn't really matter because it's going to probe and figure that out but we can enable the dry run switch and then just hit start and it will trace out in the x and y where it's going to make the cut so hit start there's the two holes and the perimeter and that looks fine program complete so i think we are ready to cut make sure i have everything switched on and i do plasma cutters happy it has air pressure so i'll turn off the dry run put on my eye protection and just hit start and that is the part i'm just going to dry off some of this water that's splashed up now this has got some dross on it from the process and we'll take that off grab my non-tinted safety glasses and i've just got a little uh battery powered right angle die grinder this is got a rolock 2 inch roll lock disc on it with a scotch brite wheel and we'll just use that to clean up the draws [Music] okay that's nice and smooth and clean and uh take this over to the sheet metal break and bend it into place and oh by the way if you were confused by the fact that there appears to already be a uh torch cover here on my torch well this isn't my first rodeo we've got the part all cleaned up and deburred let's just bend it just slide it in here underneath the magnetic clamping arm and this one i'll just align here by eye looks about right let's try turning it on and bend this up just past 90 so it'll spring back that looks about right to me that's about 90 degrees so that's the screw flange and then we need to bend up the wings on the sides and i'll do this under the front and i've got a little piece of the same material that i'm going to put under the back of the clamping bar as packing and then i have very lightly scribed a little line here where i want the bend clamp that down and i'm going to bring this up we wanted 50 degrees so i'll bring it up probably a little bit too far see how that goes that looks pretty good and we'll do the other side and that is the part complete the combination of a cnc plasma table and a bending break is a really powerful one for just quickly banging out sheet metal parts now if you add a spot welder to the mix then you've really got something special but that's a different video for a different day that's all i've got for you today thank you for watching [Music] you

Channel: Clough42

Views: 41,556

Keywords: Plasma Cutter, Plasma Table, CNC, Fusion 360, Bending, Sheet Metal, Aluminum, Langmuir, Crossfire, Fire Control

Id: FRVTYO6nvKA

Length: 30min 35sec (1835 seconds)

Published: Sun Oct 17 2021