Creating a simple part with Draft and Part WB

Introduction
This tutorial aims to be used as a first introduction to Draft Workbench in FreeCAD. The tutorial uses a 2d shape to create a 3d solid, the latter is accomplished through Part Workbench. The reader is recommended to first work through the sister tutorial Creating a simple part with Part WB, which is creating the same model with a different technique, while at the same time covering more of the basics of FreeCAD’s user interface. This tutorial expects the user to be briefly familiar with both the user interface and some workflows available in FreeCAD. The tutorial is composed such that the aim is not necessarily to show the most efficient way to use the program, but rather to make the reader aware of different functionalities available in FreeCAD, how to use them, and where to find them.

The tutorial covers

 * The model to make
 * Creating the 2d profile
 * Why does not extruding work
 * Extruding the profile
 * Creating the through hole
 * Making a sketch out of the 2d profile
 * Wrapping up

The model to make




Creating the 2d profile
Create a new document and save it directly under a new name. Change the view to Top view and switch to Draft Workbench, your screen should look like below. If the grid does not show, toggle it on/off with Toggle Grid.



To start off the profile, draw a random Rectangle on the screen in the XY-plane by clicking 2 points in the 3D_view forming any diagonal of a rectangle. A task panel will open once the command is invoked, this time we are not going to use it at all, but you could of course enter the coordinates directly for the rectangle. Your 3d-view should now have a rectangle drawn, similar to below picture.



When working in Draft Workbench one always draws on a 2d plane, that 2d plane is called Working plane, and is in default setting always automatically aligning itself to the same orientation as the current 3d-view camera position. So, until the 2d profile is completed, it is best to simply keep the TOP view (camera position) and not mock around with rotating the view. If you happened to have changed it, just change back to the TOP view before starting any new command in Draft Workbench.

The side view of our final model has the outer contour of 100 x 50 mm, and it would be nice if the lower left corner was placed in global zero position. This can be accomplished through the property-view of the created Rectangle. First change Position of the rectangle to (0, 0, 0), then modify height to 50 mm and length to 100 mm as per images below.



The Rectangle is finished and it should look like this after applying Fit all to the view.



Next we will break up the rectangle into its four edges, this is done by first selecting the Rectangle and then invoking the command Draft Downgrade, the filled face will disappear and the object in the tree-view is now a Wire instead of a Rectangle, shown in the left picture below. Invoking Draft Downgrade once more will break up the wire into its edges, shown in the middle picture below.



The observant will notice that the object icon in the tree-view already for the wire changed to a blue box. This blue box is the icon used for generic geometric objects (Part Module geometric objects to be specific, but that is for advanced readers). Select the left vertical edge and invoke the command Draft Upgrade, the former edge will now have a different icon and has changed label to Line. It is now a Draft Workbench object where one can edit for example start-point and end-point through the properties-view, this is not possible with the edge objects.

Creating the fillet
Start by selecting the upper right corner edges, use menu  Box selection, hold down the  LMB and drag from right to left and release LMB. When dragging from right to left the resulting selection includes everything fully or partially within the selection area. If one drags from left to right, only objects fully enclosed by the selection area are included in the resulting selection. The actual selection happens when the left mouse button is released, and there is no preview of what will be selected.



With the top right corner edges selected, invoke command Fillet in Draft Workbench. Check Delete original objects and change radius to 20 mm and hit.



The Fillet is created and your model should now look like below.



Creating the chamfer
To make the chamfer we need to have a line with the correct inclination and also be able to position it correctly. Let us begin with the position, which is on coordinate (50, 50, 0). In the current profile we do not have a point there, so lets create one by making a temporary help line. First select the left vertical Line, then create the help line by Duplicate selection in, Line001 is created. Use the property-view and move Line001 50 mm in x-direction using the Placement property. Next duplicate the lower horizontal edge, and change the angle of the edge to 30 degrees, once again using the Placement property. The model should now look like the image below.



Next, move the angled line into position. For this we make use of Draft Move along with the snap functionality in Draft Workbench, more specifically end-point snap. First make sure that your snap toolbar looks similar to below.



Then select the angled line, Edge001, press Move and a task panel opens up.



Make sure that Copy is unchecked. Hoover the mouse over the upper quarter of the angled line, once the white dot and end-point symbol shows at the right spot, click LMB. Move the mouse to the upper quarter of the help line, once the white dot and end point symbol appears, click LMB. The sequence is illustrated below.



The line is now in the correct position, but it is too long. To adjust the lengths of the lines Draft Trimex will be used. Click on the left part of the angled line, i.e. the part of Edge001 that is to be removed. Once the line is selected, press Trim and then click on the left-most vertical line, Line. The image below shows the Trim command invoked, and the pre-selected vertical line.



Repeat the trimming of the left-most vertical line to form the lower corner of the chamfer. Here you probably need to do the trimming in 2 steps. The trim function can make an undesired flip, keeping the longest part of the object to be trimmed. In those cases, trim a shorter distance first by simply clicking in the 3d-view for example halfway of your intended trim. The trim function accepts any click in the 3d view. If you get it wrong, just use Undo and  Refresh (the latter often called recompute) and try again.



To trim the upper horizontal edge, the Fillet needs to be downgraded so that the upper edge is it’s own object in the tree-view. If you attempt to trim it without first having done the downgrade, the trimming function attempts to trim the arc in the fillet. You will need to trim the line in steps to avoid the resulting trim to flip.

The profile is ready and shown below with the edges organized in a Group named Profile (or labeled to be precise in FreeCAD lingo), along with the help line deleted. Groups can be used to organize the features in your FreeCAD documents, it’s usage is analogue to a folder structure on a computers file system. To move things in and out of the group, use drag and drop in the tree-view.



Why does not extruding work
Let’s jump right into it, select all the edges in the group Profile, in Part Workbench, invoke command  Extrude. A task panel opens, accept all the defaults and click.



That did not work out, but it sounds easy enough to fix the error, we just need to specify a direction. Click to get back to the task panel and select custom direction.



Accept the default z-axis and once more click.



We managed to make a fence like structure, judging from the tree-view every edge is treated separately. It is not the wanted filled solid that we want. Hit Undo, and let’s try something else.

Scrolling all the way to the bottom of the Extrude task panel there is an option Create solid, check that option and click.



Everything disappeared, clearly that did not work either. Let’s go through why none of these ways are working. In the first case we got an error that the direction could not be determined. A flat face has a normal, i.e. direction, a line does not. Since from our second attempt we know that it worked when providing a direction, the error simply comes from trying to extrude a line without knowing into which direction to extrude that line. The observant will say that an arc has a normal (direction), this is true. If you select only the edge that is the arc, FreeCAD will extrude that arc, also with default settings.

In the second case it worked, but we also got an extrusion for each edge we had in our selection. The resulting features, however are not what we want, i.e. a solid.

In the third case we checked Create solid, and ended up with everything disappearing. The icon in the tree-view has a different icon as well, there is a white exclamation mark on red background, that particular overlay icon means that the feature has an error that has to be tended to. One can read up on different types of overlay icons on the wiki.

Hoovering over the tree-view overlay icon a tool tip is displayed, it says Wire is not closed.



In our case the error is not fixable. It is geometrically impossible to create a solid out of an extruded single line. An extruded line simply becomes a sheet, or shell in FreeCAD lingo. In other words, this is not a FreeCAD limitation, it is a fundamental outcome of geometrical theory. The reason why the 3d-view goes completely blank is that the created features, or objects in the tree-view, has errors in the produced shape, and thus contains nothing to render. FreeCAD does however create the new document objects (in this case extrusions) and thus hides any geometry/object used for making the new document objects. The is why the screen goes blank when trying to make a solid out of a line, or lines.

The tool-tip says it all, in order to extrude into a solid one needs a closed wire, or a face. A face is, per definition, simply a closed wire that is filled. One way to create a closed wire out of our profile edges is to select them all and apply Draft Upgrade. If applied once it becomes a wire, while at the same time it consumes the individual edges from the tree-view. If applied twice it becomes a face, either of those allows for a successful solid extrusion.

Extruding the profile
Another way to create the closed wire is Shape builder, which allows for making a wire without consuming the individual edges. Part Shape builder is a powerful tool to create any geometric entity in FreeCAD that can be used further to create complex solids from lower level entities, the simplest example is creating a line between two vertexes. Click Part Shape builder to bring up the task panel.



We can use either Wire from edges or Face from edges. Multiple selections has to be made with -key pressed down. Let’s use Face from edges, once that option is selected one can also select Planar, do that as well. Then select all edges in the profile, order does not matter (in this case) and click, and then to come back to the tree-view. The face has been created.



Select the Face and invoke Part Extrude, set the extrusion length to 30 mm and click.



Creating the through hole
To make the through hole we need a cylinder correctly positioned to make a boolean cut with.

Create a cylinder, and position it correctly. In this case the radius is 5 mm, height is made to be 60 mm. For the placement, first it is rotated -90 degrees around x-axis, then positioned in (65, -5, 15). The negative 5 in y-direction originates from that the height is 10 mm longer than needed.



It does not hurt to make the height of the cylinder longer than seemingly needed. For a simple model like this it will not matter if the cylinder is the exact height of the profile. It is however good practice to avoid co-planar faces, potentially that avoids numerical errors in the geometric kernel that can lurk around behind the scenes resulting in strange effects, or failures in subsequent operations when making co-planar faces on more complex models.

With a final boolean cut and changing appearance of the model, the model is completed.



Making a sketch out of the 2d profile
Using Draft Workbench is one way of creating a 2d profile. In Draft Workbench a wire can be made in 3d-space. FreeCAD provides another tool to make 2d profiles – Sketcher Workbench. Using a sketch to make a 2d profile is a more versatile way to create a 2d profile. Any 2d profile made in Draft Workbench can be converted to an unconstrained sketch.

Start by hiding the Cut feature and make the edges in the profile visible. Select the edges in the profile from the earlier made group Profile. From Draft Workbench press toolbar button Draft to Sketch and you should see the same as in the image below.



Next, hide the original edges and double-click the Sketch object in the tree-view, bringing you to the following state, i.e. the sketcher task panel opened.



This is how it looks when one edits a sketch. Since this is not a tutorial for using the sketcher just go ahead and close it. If you want an introduction to sketching, which is a core workflow in any 3d parametric cad, please follow the sister tutorial Creating a simple part with PartDesign.

With Sketch closed and selected, from Part Workbench use Extrude in the same way as for the earlier extruded profile Face. The basic block of the simple model is ready once again.



Quality of models
Sooner or later when working with 3d parametric cad you will come across a broken model, either one you have made yourself, or a model that you have imported. A broken model can work for its purpose, but more often than not, there are subsequent operations that simply will not work with a broken model. To repair a broken model one has to know what to repair, this is where the built-in quality check tools in FreeCAD come in.

First let us check the quality of the recently created Extrude001. With Part Workbench active, first select Extrude001 and then use command Check geometry.



Our model is OK, no errors are reported. There is also a listing of the models content, or in FreeCAD lingo, the content of the shape, i.e. how it is put together from ground up. Here one can see that apparently to make a solid one also needs a shell, and the shell is made out of faces, and so on. In other words, you can create any solid by simply starting out by making points, or vertices, from those one makes edges, and from those one creates wires, and out of the wires one makes faces which are then stitched into a shell, from which one finally arrives at a solid. A solid can only be made from a watertight shell. A not watertight shell is a common source of troublesome cad-models, it can for example happen with imported geometry created in a different software, especially when using the commonly available neutral file formats.

One other check one can do is related to the Sketch. Close the task panel for the geometry check. Select the Sketch, expand Extrude001 in the tree-view if needed in order to see the sketch-object. Switch to Sketcher Workbench, use command  Validate sketch, a task panel opens. In the task panel, click the button for Missing coincidences. It highlights and reports 6 of them, i.e. all the points where the edges meet.



Click in the pop-up dialogue and then click the  button  to heal the Missing coincidences. If you close the task panel, and go into edit mode of the Sketch, it reports 12 degrees of freedom, as opposed to the earlier 24. That was achieved through adding coincident constraints to the endpoints of the edges. The observant reader notices that when using edges from draft those had to be joined into a closed wire to make a solid extrusion, whereas in sketcher that was not apparently needed. The logic here is that the sketch is one object, and the extrusion of one object is treated as if it was a closed wire (in this case).

Finally it should be pointed out that although it can work creating subsequent objects with open vertices in sketches, it is best practice to not have any, as well as having a fully constrained sketch (as opposed to an under constrained ditto). The reason why it works here is that the sketch is created from a profile that has all edge endpoints matching without any gaps, since it is originating from a draft profile where it has been constructed in such way that exact edge endpoints matching is ensured (for example by use of snap). If you in the sketcher draw by hand and also try to match endpoints by hand, it is virtually guaranteed that the endpoint will not be matched from the sketch solver point of view, i.e. the gap (although not really visible on the screen) is large enough that the geometric kernel cannot consider them to be matching endpoints, i.e. edges are not geometrically joined.

Wrapping up
Having gone through the tutorial you have become somewhat familiar with the basic functionality of FreeCAD, along with the core workbenches Part and Draft. You are also aware of the existence of Sketcher Workbench, which for many experienced users is the sole tool used to create 2d profiles later utilized in solid feature operations. The use of sketches is a core concept in PartDesign Workbench. It is suggested that you learn sketches and PartDesign Workbench next if your focus is on creating solids. The sister-tutorial Creating a simple part with PartDesign makes the same model as this tutorial. If your focus is modeling buildings your next learning should be the Draft and Arch workbenches.

At last, FreeCAD is made by volunteers in their spare time. If you want to further advance FreeCAD’s capabilities, consider contributing to FreeCAD, for example by improving documentation.