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FreeCAD - 3d design tip, tricks, questions and hopefully answers!


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Following on from @danny_galaga's thread over here, I've decided to give FreeCAD another try. I'm currently using 0.19.3 - available for free here https://www.freecadweb.org/downloads.php

I have been using Autodesk Fusion 360 for my 3d design for 3d printing until now, but they keep changing their licencing arrangements, and I'm concerned that their free offering won't be free forever. With that in mind, I'm set on learning more about FreeCAD, and hope to share some tips I've learnt along the way - maybe others can chime in, and maybe some can learn a thing or two. Feel free to post any questions or requests for designs in here, and we can see what we can learn together!

First cab off the rank was @danny_galaga's request for a flying saucer shape as per the specs in this rough sketch:



We'll kick off by going into the 'Sketcher' workbench to draw that side profile he drew.


We want to create the sketch in the XZ plane as that allows us to define the shape's height and width, before we create the depth.


One trick I learnt early on was to grab this 'Sketcher Constraints' toolbar at the top, and drag it onto a second row of the toolbars. This allows you to get access to all of the constraints you'll need to make a good complete sketch.


Start by drawing the shape you want - in this case it's just with straight lines, so fairly straightforward. At this stage don't worry about trying to get the lines the right length, having them exactly at right angles etc


Ok, now the basics are in there, we need to constrain the sketch so that it's to our exact specifications. This includes measurements, making sure our diagram is on the axis, making sure lines are horizontal / vertical as required, and making sure all the points are joined together. I'll run through the extra constraints I had to add in to make the final sketch - you click on the line, then the constraint button from the toolbar to create it. Once they are all done - the whole diagram will be lime green saying it's all good to go. When things aren't all constrained, you can grab lines and points and move them freely, but when they are all locked in you know it's designed how you want it to be:

image.png.15bdcc702826adf40ff597bb119eef54.png Vertical constraint - make the line only run up and down! - when I drew the bottom right line it wasn't straight, so added one there

image.png.d7805aa50c0d790884c46eb2f8c648af.png Horizontal distance constraint - used to set the measurement of a line - or distance between points. I used this to set the 10mm line at the bottom, 0.5mm line at the top, and the 5mm distance between the bottom lines left most point, and the origins point.

image.png.cd88c45e85d379ed4172bdaf5669a809.png Vertical distance constraint - as above for setting a measurement - but for vertical distances. Used to set the left line's length to 3mm (mentioned as the height in the original thread) and the right line to 0.4mm.

And there we have it, one nice green sketch!


You can see over in the left under the Tasks section that the sketch is fully constrained. As you work through the constraints it will show you how many 'Degrees of freedom' are in your sketch - I like to think of these as things that need to get fixed before it's locked in. Click on the Close button.


Now we swap from the 'Sketcher' workbench to the 'Part' workbench to make it 3d



Since this part is a circular object based on this side profile, we want to use the 'Revolve' tool image.png.75766810f9c375a870e837f964e03cf7.png. To select this, you'll have to have clicked on the sketch on the left, then click on this button. Once clicked on, the following will show up on the left. The defaults are ok here as we want to Revolve it 360 degrees, and not change any of the centre or offset values, but if you only wanted say 180 degrees, this is where you'd do it.


Clicking Ok does the Revolve - and we're done!


For 3d printing, you can select the part (named 'Revolve' as that was the last action we did) on the left side, then click File->Export, and you can save it as an STL file, load into your favourite slicer, and you're away!

To make some tweaks to the part, you can expand the steps we've been through in the Model browser on the left. Double clicking the Sketch here will open it up, and you can edit the constraints in your model as required (say you wanted the hole in the middle to be 5.5mm radius instead to allow for the tolerances of your printer)



I've attached the design file for those that want to just jump to the end and play around with it from where I got up to.

Next time I'll walk through making the teardrop shape Danny referred to - the 60mm long part of his sketch!



Edited by Zzap
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Ok, example number two was to make a teardrop shape similar to above - in the original sketch the total length was 60mm. To make this kind of shape it seems that the 'Loft' tool would be best, this is where the 3d tool will join the lines from one sketch to another, filling in the sides to make a solid object.

First up, as above, we start with a rough sketch in the Sketcher workbook - again in the XY Plane.


After drawing this in roughly (without specific dimensions), we again need to constrain the diagram.

image.png.bb7c6b57dcedd42a465d308668c7d1e6.png Tangent constraint - used to make a line run tangentially to a circle or arc. This will mean that our straight lines will run exactly into the circles and make it neat. I had to add 4 of them here, 2 onto each of the lines, added to each of the circles.


image.png.119951fe520f211997ea115228064ca7.png Radius constraint - this sets the radius for a circle or arc. In this case I set the left circle to be 15mm radius as per the diagram, and the right one to be 5.5mm - as that seemed about right - it can be tweaked later!

image.png.7c4c344379acae258f6f7f926b2a0dc4.png Distance constraint - this was used to set the distance between the centre point of the left circle to the centre of the right circle. One trick here was we know the total distance from the leftmost point to the rightmost to be 60mm, so and we know the radius of the left and right circles are 15 and 5.5, so we can actually click on the little formula (image.png.bbd371c5139eef77383f882e031e7ed9.png) symbol - and enter the values "60 - 15 - 5.5", and it will do the calculation to make it 39.5


Here we are now locked in and all green for this sketch!


From here we need to make this just an outline of the base, so we need to get rid of the two inside arcs of the circles. Clicking on the Trim tool (image.png.6211bbbf602c6a81765ae4b00cfe6835.png) and then clicking on the arcs they will be deleted, and we're left with just the nice teardrop base shape.


We click Close over on the left, then it's time to create a new sketch for the top of the saucer. Click on the new sketch button (image.png.d63c0e80303d44d1ec3f88877853a497.png), and this time we are going to make a new sketch in the XY plane, but offset by 3mm to represent the thickness of the object:


So this new sketch will be parallel to the last one, but 3mm up in the air. For this new one, it's a nice simple single circle, with a radius constraint of 5.5mm.


Clicking Close again after constraining that sketch, we can see the two sketches, offset by 3mm


From here, we click across to the 'Part' workbench, and we can click on the Loft (image.png.f4245e25e9199bdebe6028fdccc79e6b.png) tool to create an object between these two sketches. In this window that pops up, move the named sketches from the left to the right to include both, and make sure to tick ‘Create Solid’ at the bottom before clicking ok.


Voila, one teardrop saucer!


At this stage some of you playing along at home might have thought “Zzap, he wanted it to be 3mm high, but that included 0.4mm band around the base” – yep, at this stage I had forgotten that measurement, but don’t worry, I’ll show you how to fix that up too… Over on the left in the Model browser, you can expand our nice new loft, click on Sketch001 (this was the second one we created), expand the Placement->Position, and you’ll see the 3mm offset there. Since we want 0.4mm taken out of this bits height, we can adjust it here to 2.6mm.


Click on that, change it to 2.6, hit enter, and it’s locked in (if you watch the 3d model, you’ll see it get a little shorter)


While we are in here, lets extrude that 0.4mm band by clicking on ‘Sketch’, then Extrude



Not that that's -0.4mm because we want it to go down from where the sketch currently is, click Ok. Now we technically have two parts, we can merge them together into one by clicking on the 'Loft' part, hold down Control Key, and click the 'Extrude' part, then click on Union (image.png.fdb2b5ac2a5520b4b260110bb1eb132e.png). And we've got one part now with the 0.4mm base:


Now to move onto cutting out the 5mm radius hole down the centre. Clicking on that flat circle (green above), and changing to the 'Sketcher' workbench, we can create a new sketch on that face:


Now draw a constrained 5mm hole at the centre point:


Click Close. Now swap back to the 'Part' workbench and we're going to extrude that hole. Click on the newly created sketch in the Model browser (Sketch002), and then click the Extrude button (image.png.2912b211dd5d57dd79e54c42af1c69e3.png). We want this hole to go the whole way through from where it is down, so we need it to go -3mm:


Clicking ok, we can see the new extrusion - easier if we hover over it in the Model browser - its name is Extrude001


Now to take this hole away from our previously created part, we use the Cut (image.png.373cbe52747cc439bf2ef85379bf5329.png) tool. In the Model browser, click the part 'Fusion' and 'Extrude001', then click the Cut too, and the Extrude001 shape is cut away from the Fusion shape, leaving us with a teardrop saucer, with a 5mm radius hole in it!



FreeCAD model has been attached for anyone interested, and if anyone else is keen to learn more, throw some questions in here and let's see if we can get them answered! If anyone else is in need of a part 3d modeled like this, also ask away and I'll see if i can make it happen! I'm definitely not an expert on this, so if anyone sees anything that could be done better, please help us all out and chime in :)


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Yeah, there is a lot of these different 'Workbenches' in FreeCAD that I'm not quite sure how they all interact yet, but keeping just in Sketcher and Part seem to be working for me so far! There's the Draft and Part Designer that seem to do similar things, but Sketcher and Part just seemed to work for me so that's where I've landed for now.

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