FreeCAD Basic Exercise #4
This tutorial introduces the Construction Mode for constraining sketch geometry and also new features: Polygon, Equal and Fillet (in Sketcher) then Thickness and Polar Pattern (in Part Design).
Step 1: Presentation of the exercise
We will model the part illustrated below by the method proposed in the tree structure.
For the dimensions of the part you can refer to the drawing below but they will be repeated in the modelling procedure.
Step 2: Modelling procedure
1. Create a cylinder with a diameter of 150 mm and a height of 20 mm with the functions Circle (coincident with the centre of the marker) and Pad.
2. Create three circles of the same diameter, equidistant and centred around the axis of the cylinder following this steps :
A) Activate Construction Mode and select Polygon → Triangle to make a construction triangle centred on the cylinder axis.
B) Place a horizontality constraint to align the height of the triangle with the marker.
C) Turn off Construction Mode and then create three circles coincident with the vertices of the triangle.
D) Create an Equality constraint between the three circles.
3. Add diameter constraints of 35 mm on the sketch circles and 75 mm on the construction circle.
4. Apply the Pocket function "Through All".
5. Click on the top face and use the Thickness function with the following settings: Layer (default setting), Intersection (to keep sharp edges) and Generate thickness inwards (to shift the faces inwards).
6. In a new sketch, create a triangle with rounded edges using the Fillet function. The triangle will then need to be connected to the construction circle and an arc constraint created as shown below.
7. To keep the holes open, create a Pocket by selecting the circular faces at the bottom of the holes
8. Create the sketch below with the Arc and External Geometry functions. Apply a 5 mm pocket.
9. Use the Polar Pattern function on the newly created pocket with an angle of 360° (default) and a number of occurrences of 3.
9. Add edge fillets to finalise the part.
Thank you!
Thanks to you! It's always nice to get feedback :)
This exercise is very difficult. Thank you :)
Thanks for your feedback Vinicio :)
There is an instruiction missing between step 5 and step 6 to flip the part over before creatiing the sketch in step 6. This would have prevented me from having to do the exercise twice. But I learned a lot...
made it through! I can't tell if you left out detailed steps to challenge us to figure it out, or if a few more details would help on step 6 and 9.
Looks awesome! Thank you for the polygon detail!
I learned a lot again Quentin.
Many thanks.
In version 1.0 the icon for 'Construction mode' has changed.
It is now a line with a dashed line above it and is now called 'Toggle construction geometry'.
Hello. Thank you for your tutorials.
Can you give more step by step details on the #6 ?
I am using freecad 1.0 and I am stuck. Is it possible the same way ? How do you do the "The triangle will then need to be connected to the construction circle" ?
I had to give up at step 6 - too many unknowns for me. Maybe also the screenshots were too small so i missed out on key information? My main questions are: do i create a new sketch on the XY plain or on a face of the shape already created? Do i flip it andy why do some parts seem to be placed on top of the sketch when i create a new one? Ihave enjoyed your tutorias so far, but this was the point that got too hard for me. Maybe i will get back, when i have learned some more, and may can see what i made wrong. Also some features have changed name since this was made, so users need to check the wiki to figure out what they are called now and what the icons look like. Thanks for the tutorials anyway! i learn a lot!