How to use the Additive Pipe Tool in FreeCAD's Part Design Workbench

today we're going to look at the additive pipe tool which is part of freecad's part design workbench stick around [Music] [Applause] hi i'm jeff and i'm going to help you learn free cad so you can design the things you've imagined if you're new here don't forget to subscribe to the channel and click the notification bell so you stay up to date with my videos the additive pipe tool allows you to create a solid from one or more sketches that follows the path that you've defined the additive pipe tool is also known as the additive sweep tool in this video i'm just going to refer to it as the additive pipe tool for consistency i've created the sketches that i'm going to use in the demonstration beforehand so that we can concentrate on the tool itself if you'd like to support the channel you can buy me a coffee through the link in the description below all donations will be used to help improve the channel now let's get started i'm using freecad version 0.19 built on the 26th of feb 2021 for this demonstration and i'm running it on kubuntu linux i have a keyboard and mouse display in the bottom left corner of the screen and that will show you the mouse clicks and hotkeys that i use i'll normally say which hotkeys i'm using but just in case i don't they'll show up down the bottom in the keyboard display let's have a look at the basics of the additive pipe tool i've created a drawing that has some simple sketches in it and we'll use those to demonstrate the basics so in the first example you can see i have a simple pipe that curves around a 90 degree corner one way you can start the additive pipe tool is to click the icon without having any sketches selected so we'll do that and then what you do is you select the first sketch which in this case is the rectangular section of the pipe and then you click the ok button and then we select the path that we want it to follow by clicking on the object button and then selecting the path you can see that the tool creates the pipe along the path that we just followed so we'll cancel that and we'll look at the next way of starting it the next way to start the tool is to select the sketch and then click the icon then you just need to select the path that you want the sketch to follow so we click the object button again and select the path the next way to start the tool is to select the sketch and the path make sure you hold down the control key while you're selecting each of the items so we select the sketch and then the path that it is following and then we click the icon and you can see it's created the pipe now that we've looked at the basics of the the tool it's time to dig a bit deeper and look into the options as well the first pipe that we created was a simple rectangle that followed the path i've previously created a sketch representing the slot and i will enable that now i do that by clicking on the sketch and then pressing the space bar to create the pipe that transitions from a rectangle to the slot firstly i will select the rectangle and start the tool and then i will come down to the bottom of the task view into the section that's entitled section transformation and i will change the mode from constant to multi-section and then i'll add the slot by clicking on the add section button and then selecting the slot and then we will just select the path as we normally do by clicking on the the object button and selecting the path itself as you can see if i rotate this around we start off as a rectangle and we finish up as a slot now we'll look at an example where you can add multiple transition sketches to a pipe in this example the pipe will start as a circle then transition into a hexagon and then finally transition into a square i'll start by selecting the circle and then starting the additive pipe tool i will then add the path [Music] and then again we'll come down to the section transformation and change that to multiple section and then add the first section being the hexagon you can see that it's already started to change and then we'll add the final section which represents the square and now we have a pipe that starts as a circle transitions through a hexagon and finishes up as a square this is not a particularly practical example but it does give you an idea of how you can use different sketches to produce the pipe that you need keynote viewers will note that we haven't yet looked at the section orientation options so let's do that now i'll continue to use the multi-transition pipe to show you these options the default option is standard and this keeps the cross-section of the pipe perpendicular to the path the next option we have is the fixed option the fixed orientation is set by the first sketch in the pipe and is applied to all the subsequent sketches along the path as as you can see switching between standard and fixed changes the shape of the pipe significantly the frenetic option reduces the amount of twisting that occurs in the pipe this is not something that i've used in my work but it appears to be useful when your pipe has many twists and turns in it creating furniture components that have twists and turns is not impossible but i've not done it nor ever had a need to do it so i'm not sure that i will ever use this option the next orientation is the auxiliary orientation and i'll come back to that one shortly the last orientation is the binormal orientation this orientation allows you to specify a binomial vector i've set the vector to some random values just to show you that it can affect the the pipe the binomial orientation seems to affect those parts of the pipe that are following a curve this is not something that i use in my work and to be honest i can't see a use for this orientation but i'm sure there must be a reason for it if you've got any examples of it please let me know in the comments below now we'll come back to the auxiliary orientation and have a look at that in the examples that i've shown you so far i have just used a path that is defined on a single plane but what happens if you need to design a pipe whose path is defined by several planes well this is where the auxiliary orientation comes into play now i've created another example which we can use to show you that in this example i've created two circular sketches that represent the start and the end of the pipe and i've also created two sketches that represent the path that the pipe will follow each of the path sketches is defined in its own plane and they will be combined to produce a single path that crosses both those planes pipe is created in the usual manner so we'll select start and then we will select one of the paths as you can see it has created a circular pipe along that first path now we will change the section orientation to be auxiliary and we will also then select the other path that's defined in the model and you can see that it has changed the created path in this case i think it's fair to say that it's sort of mangled it a bit the last thing i'm going to do in this example is change the section transformation to be multi-section and add the end sketch and you can see that again it has changed the shape of the pipe that it has produced it has compressed it as it's bent it now it's also fair to say that this is not a very practical example the paths i've used in this example did not give me the result i was hoping for but they do show how the paths influence the pipe that was produced is there a way that we can produce a better pipe yes there is so just close this one down i used curved workbench to produce a curve that was defined by both the paths used in this example the resulting path gives me a pipe more like what i was expecting i will create another video showing you how to use the curves workbench to produce this sort of path but for the moment i will just enable the path that i've created so you can see it i will hide the two paths used to create the curve and then we will create a pipe using that curve the curve produced by the curves workbench is not compatible with the part design workbench so i'll need to introduce a shape binder which will allow that curve to be used with the part design workbench i'm not going to go into detail about the shape bender that will be the subject of another video we'll click on the shape bender icon and then we will add the curve and click ok and now what we'll do is we will create the pipe as we normally do so we'll select start sketch create the pipe we will sweep it along the shape binder and then we will put the transform mode into multi-section and add the last section and then we'll turn off the curve so we don't have to see it now this is more like what i was aiming for but you can see that it's not as smooth as i would have liked but it also does show that it is possible to produce a nicer curve across multiple planes i've been talking about using the additive pipe tool to create solid pipes but you can also use it to create a hollow pipe i've created a sketch that shows this as you can see the sketch is just two concentric circles with a small gap between them now when i create the pipe you will see that the result is hollow [Music] i can't see how this would be useful for woodworking but can see that it could be useful in other fields of engineering so far we've looked at how the additive pipe tool works but it also has a number of limitations that you might come across during your work let's have a look at them the sketches defining the profiles must be closed this seems obvious to me but perhaps it's not to others the tool creates a solid from the profiles so having an open profile doesn't make any sense to me let me just show you that now [Music] i find it interesting that the error message seems to indicate that you can use opens profiles for the start and the end let's just explore that so i'm just going to cancel this one i've created another sketch for the opening profile which i will just activate now and disable the closed one let's try making a pipe from that based on everything that i've read about the additive pipe this is the error i was expecting i'm not sure why the other error message would suggest that you can use open profiles but obviously you can't the next limitation is that the path cannot contain branches or t-junctions let's explore that [Music] initially this didn't seem to be obvious to me but i hadn't really given it a lot of thought in hindsight it does seem obvious i think to solve this problem you would need to create two pipes and then merge them together i'm not going to do that at this point stepping away from this specific example it should also be obvious that you cannot use a vertex to define the profile this would simply give you a pipe that is the path itself with no size or mass the next limitation is that the path can only consist of a single sketch so if you need more than one sketch you're out of luck or are you let's have a look in this example i've created two sketches so there's path one here and path two here so what i'm going to do is we'll just basically start with a additive pipe as we would normally do and then we'll try and add the second sketch and what you can see is that it makes a complete mess of the pipe that i was trying to create so the solution to this problem is to use what's known as a subshape binder so what we do is we select both sketches and then we start the subshape binder tool what this does is it creates a binder of the two so if when i click on that you'll see that it's encompassed by sketches so what we do now is we select the start profile and the binder and then we create the additive pipe and that works as you'd expect if however you just select the start profile go to create the additive pipe and then select the path we'll get the same problem we had before because it doesn't select the subshape binder so we need to make sure we click in the model we need to select the start profile and the binder before we initiate the additive pipe tool the freecad documentation recommends that all profiles have the same number of segments to produce the best result i'll use the example of a square transitioning into a circle to demonstrate this so as you can see i've got my start profile and i've got my end profile which is a circle made up of a single segment so if i create the additive pipe using those two profiles you can see i get a a pretty strange looking pipe nothing what i was expecting so if i delete that and disable the single segment circle and then enable an end profile made up of multiple segments which i'll just show you now as you can see it's got four individual arcs covering 90 degrees now when i create the additive pipe [Music] you'll see that i get the result i actually expected where each edge of the square transitions into a corresponding edge segment on the circle and that happens on all four so we get a much smoother and better pipe so you can see the additive pipe tool is quite a powerful tool i think it can be used in woodworking projects when you're looking to include bent lamination or steam bent parts in your furniture but outside those scenarios i think it has limited application in woodworking it seems to me that this tool could be used in other fields outside of woodworking in particular i think it could be quite useful when it comes to 3d printing i have limited experience with this so i may be mistaken your mileage may vary well i hope you found it interesting please click the like button if you liked what you saw please leave comments topic suggestions and questions below if you'd like to support the channel you can buy me a coffee through the link in the description below thanks for watching and we'll see you next time

Channel: Glasson Design Studio

Views: 14,351

Keywords: freecad, freecad part design, freecad 19, part design, freecad 0.19, freecad part design workbench tutorial, freecad part design workbench, freecad part design sweep, freecad 19 ubuntu, freecad part design tutorial, freecad 19 tutorial, freecad drawing, freecad tutorial, part design freecad tutorial, part design freecad, furniture design using freecad

Id: 2UglQ2hurS8

Length: 17min 8sec (1028 seconds)

Published: Sun Mar 28 2021