3D modeling FreeCAD Tutorial - Loft modifiers!

hello and welcome to another tutorial with me andrew today we're going to be taking a look at the loft tool in freecad so the first question what is a lot tool well the loft tool creates a 3d solid or surface in space between multiple cross sections which flow and blend into one another take for example this door handle what looks to be complex geometry is actually just three separate sketches so where is lofting normally used well it can be found in complex natural geometries such as a vars a variety of household bottles door handles in fact most things that are hand out probably have some form of flow surface which can be created with the loft modifier how do we actually use the loft modifier well the first one i'm going to show you is going to be in the part design workbench and it's called an additive loft this can be found up here on the tool ribbon next to the revolve sketch icon so let's actually create this door handle using the loft modifier so i'm going to create a new document create a sketch and i'm going to place that on the x y plane i'm going to grab the slot geometry click on our center point and move it out shift v or shift h sorry which will then be able to constrain our horizontal to 10 mil and i'm going to constrain the radius to 5ml i'm going to close that and with our sketch selected i'm going to create a datum plane we're going to set the pitch to 90 degrees and we're going to set the x to 50. so what i should do is move our plane in right direction and it should also orientate it like so i'm going to click ok i'm going to click on the data plane create a sketch and i'm going to grab the circle tool i'm going to click on our horizontal or vertical line in this sense and i'm going to set the radius of that to three mil pressing shift h we're going to click the center of our point and click our origin point we're going to set that to 15mm i'm going to close that hide our datum point and i'm going to create one more sketch which is also going to be on our x y plane now this is going to be exactly the same as our slot tool here and it's just going to be on our horizontal 10 mil apart and with a radius of 5 mil [Music] i'm also then going to set the spacing between both of our slots so from the origin point to the center point we're going to set up to 90 mil and we're going to say okay and close that so now we've got our sketches and as you can see it's in this sort of layout what i'm going to do is now i'm going to create the additive loft so i'm going to select our first sketch and click the additive loft i'm going to click on add section and the reason why i click add section first is because if i say if i click circle it will then create the loft but if i was to click the sketch and then click add section it wouldn't actually add it it needs me to click add section first and then click the actual sketch so as you can see it now creates this curve so it's actually blending from each individual sketch uh to create the handle as you can see so a couple of things you need to know so number one it will always create a loft from the first sketch you select and then afterwards so if i was to remove this selection here and then add this selection again it would create some sort of random spawn of evil mainly because of how we've selected it so we've selected in a sense this sketch moved over and selected this sketch because we just deselected this and then we've selected this one again and as you can see it's created this if i remove this sketch remove this sketch and add the sketch here and then add this one again it then creates our loft in the correct order or the order that we actually want it to be so obviously we've got a curve here so what happens if you don't want a curve well that's where raw surface comes in so raw surface basically picks the uh it basically creates a straight line to the geometry that you actually want as you can see it's going from one spot to the next ball without the curve so if we take that off again it will it will give us a nice curve closed is something i can't actually work out at the moment i haven't actually managed to get it to work properly but basically what that would do is it would um go from if it can or with freecad can it will go from the last point you selected and it will try to reconnect itself back to the beginning point basically so i'm guessing most geometry or the geometry has to lend itself to being that um which our geometry doesn't our door handle doesn't but yes that's basically what that is so i'm going to click ok and that is now going to create a solid object like so so this solid object can actually be pocketed if we wanted it to so if i create a circle just very roughly there and i clicked the pocket icon as you can see i can still actually modify or edit our part next we're going to quickly look at the subtractive loft which can be found here next to the grooving tool we'll quickly create ourselves a cube and leave all the settings as their default values i'm going to select the xy plane just out of habit and i'll set the view to isometric so i can see it better and create the sketch on our top face i'll take the polygon tool and roughly sketch it on the center of our cube i don't need to constrain this as it will work anyway if you're creating something that needs to be accurate then obviously make sure it's the size you want clicking on our top face again or our sketch doesn't matter which i'm going to create a datum plane and set the z offset to minus 5. i'm going to increase the cube transparency so that i can see what i'm about to sketch and we'll now create a simple circle on our datum plane that we've just created roughly in the center of our polygon like so hiding the dating point again just out of habit is not necessary but just makes things easier to see and less cluttered so i can select the polygon sketch however if i don't i'll be prompted to do so when i click the subtractive loft icon and that goes for the additive loft also sketch selected i'm going to quickly double click the cube and hide it so i can select my circle geometry as you can see i can't currently do that make sure to hide it while in the loft modifier because if you hide it before starting the loft it will just reappear the raw surface and closed tick boxes are the same as explained earlier although if you're creating a loft between only two sketches it will automatically be ruled we have a pocket in our part created by a subtractive loft so what if we want to modify the sketches well the great thing is we can let's say i want this circle to be a square i click on the circle sketch and create myself a square the loft updates automatically what about the square being off center you can do that too again the loft will automatically update i can also click on this face and extrude it through the whole cube without any issues using our handle for reference i'm going to delete the additive loft and make all three sketches visible again moving over to the part workbench we have the utility to loft which is on the ribbon here if we click it you'll see that we have two sections available profiles and selected profiles you'll also notice that we have both road surface and closed tick boxes along with a new one called create solid so to quickly show you i'll click the first sketch and the right pointing arrow now becomes clickable you can't select multiple sketches so you'll have to move each sketch individually i'll click it and this will move the selected sketch into the selected profile box if i then select the other sketches and move them across you'll see that more arrows become available i can reorganize the order of our loft which as i mentioned earlier is very important and we can also move the sketches back into the left hand box by clicking the left arrow if i tick the create solid box and say okay it will create our handle in solid form similar to the additive loft however it will create a separate entity which can't be modified unless you go back into the part workbench and create a new body with that loft so about if you don't click the create solid box in this case it will create a surface like so now you can attempt to create a body from a surface of which you'll get a warning box like this so i'll say use that at your own risk because i'm not really sure what the outcomes will be or whether the part will become buggy i'm still not sure what i'll personally need a surface for however it's there if you need it continuing with lofting just a surface i've created two simple arcs again not constrained and with a datum space 20 millimeter from the bottom sketch i'll click the utility loft stick across both sketches and hit ok this will now create this flowing surface if i clicked create solid it would still work but it just won't create a solid form to create a solid the sketched cross sections have to be closed i can now go into the part design workbench and extrude this face once you create the extrusion it will become part of the active body which can then be edited just be aware that sometimes it can turn black and totally bug out probably because you aren't supposed to be doing this but i'm showing you because it works and you know you guys can make your own decisions last but by no means least how to connect a sketch to a piece of existing geometry i've got this piece of random geometry which i've created with a polyline i've then offset a datum plane 10 millimeter from the bottom face and created this circle sketch now what if i wanted a loft from the sketch to my part or vice versa well in this case the sketch is available to loft which makes things very simple as you can see but if there's no sketch available and the geometry is too complex unfortunately we can't loft directly to a face it creates an error like this it would definitely make things a heck of a lot easier because you wouldn't have to keep jumping to different workbenches so how do we get around this problem the answer a face binder face binder basically maps a selected surface and allows us to loft to that shape so we head over to the draft workbench and select the face we'd like to loft to we then go over to the face binder icon which is up here and click in our tree to the left we now have an item labeled as a face binder now we can either use an additive loft in the part design workbench or a utility loft in the part workbench for this i'll use the part workbench we select our loft modifier select the sketch we require in this case it's this one because we are pretending that this doesn't exist move it over to the right then select the face binder and do the same we'll click create solid and press ok as you can see we've now lofted from a sketch to a solid bar just be careful how complex you make the geometry because as you can see from this b-spline part it gets a little confused with what i've created hopefully i've given you something else to experiment with this weekend i would love to sit here and show examples of what you can create but that would be a very long youtube video have yourselves a mess around with the loft modifiers and just get comfortable using them they're definitely a great addition to the freecad toolbox if you like the video then give it a thumbs up if you dislike the video then give it a thumbs down thank you so much for watching i really appreciate it i've been andrew you've been epic and i'll see you in the next video

Channel: Andrew CAD

Views: 15,874

Keywords: FreeCAD, Tutorial, Learning, 3D design, design, 3D, Design engineer, design engineering, engineer, CAD, Quality, how to guide, create, how to, Sketch, datum, detailed, version, 0.18, 2020, learn, how, to, howto, explained, sketch, workbench, part design, tools, module, loft, tool, freecad, cad, modifier, utility loft, additive loft, addative, subtractive loft, education, educational, descriptive, surface, surfaces, creating, ruled surface, facebinder, draft, part, how to use, Freecad drawing, plan, geometry, plane, constrain

Id: jP5dCB6FDpo

Length: 11min 47sec (707 seconds)

Published: Sat Nov 14 2020