3d printed housing for brewing thermostat

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c64club
Posts: 2
Joined: Sat Jan 18, 2020 2:21 am

3d printed housing for brewing thermostat

Postby c64club » Sat Jan 18, 2020 3:50 am

Hi all,
it's my first post on this forums. It's also my first "project" in Freecad that was finished and used in practice. Housing contains two pieces, modelled as two bodies in Part Designer. Front with flexible "keys" to push switches on PCB, and back with "eyes" to mount on wall. Both parts are screwed together with four small screws that keep PCB between. It was printed on Prusa MK3S printer and required only threading by hand. I made two completes. Will post a photo as soon as I connect everything together.
termostat.png
termostat.png (258.96 KiB) Viewed 1420 times
Thermostat itself looks lie this:
w1209.png
w1209.png (202.41 KiB) Viewed 1461 times
Now I live in Antarctic Station. In windy days I have some free time and decided to finally learn to use FC. In past 6 years I tried to do it, but each time I ended by moving back to modelling in Inventor.

Some parts of work done on my laptop with FreeCAD 0.18 AppImage (thaaaanks for appimage version) running on Linux Mint 19.3. Some other on colleague's PC with Win 10 and FreeCAD 0.18, just to find differences, if any. Both FC instances work the same way, without crashes. Only one issue - something hen I opened the project file back on Linux, after making key labels on Windows machine I had to delete last fer pads with their sketches and remake them.

But finally I have two shiny enclosures made from orange and red plastic.

Am I doing everything wrong? Didn't find any method or even a tip in user's documentation or in tutorials. What was most difficult for me:
1. Sketcher tool:
- rectangle with rounded corners had to be drawn manually, constraining fewteen things by hand, instead of just picking start and end corners.
- Copying "keys" shapes. They are made by cutting narrow pockets in front wall. First one (SET) Was drawn with polyline (upper half), then copied with mirror to make this symmetrical shape. I had to reconstrain everything in copied part of drawing. Second one (Minus) was done by "Create symmetric geometry" from first one. But why? Why? Why there only the lines were copied, without constrains (only few, probably randomly chosen, constrains left)? It's not a bug/lack, it's a feature, I said to myself :) I reconstrained everything one more time. With third key (Plus) I was close to to abandon the idea of making this housing on computer ("Maaaan, it takes 10x time that it's worth. Just get some plastic box laying around, cut it a bit with file and you are ready"). I found no way to just rotate copied fragment of drawing. There were two options. One was to redraw all the shape "vertically", second was to "create symmetric geometry" reflected by line of 45* angle. Both are bad and stupid, but I haven't found any reasonable alternative for them. So finally the middle key was redrawn. If I had to make 7 keys in different places and by different angles, I would turn off the computer.
-Dimensions. Every dimension had to be typed manually. Ok, I can constrain few lines with "equal" lenght then define lenght for only one of them, but I can't give them a dimension by just derive the value/size of eg. radius of existing circle.
-If I typed some equation in "dimension" textbox, only the resulting value was saved to drawing. No way to make some rectangular hole just "2.5 times bigger than other existing dimension in project, eg than wall's height".
-didn't find a way/tool to clone some closed shape in different size
2. Fillets and chamfers:
-no option to chamfer/filet an internal corner, to make something similar to "corner weld".
-no option to make 1mm chamfer on egde of 1mm thick wall. Had to make 0.99mm. No option to chamfer through two pads.



I've designed this housing on paper and only modelled in FC. All my previous FC attempts always ended in moving back to Inventor(TM) because of lack of time for hand operations (or for learning curve). Althrough I kept my fingers crossed for FC since I saw it first time in 2013. For Inventor user, FC looks like a big, fuel efficient, sophisticated excavator which can automatically search for coal, but requires some measurements and hand shovelling before each small movement of backhoe :)

Great respect fot all you FC team for developing such a big tool as a hobby project. And for all you users for designing your complicated projects and sharing solutions for many things.
m0n5t3r
Posts: 98
Joined: Fri Feb 03, 2017 2:55 pm

Re: 3d printed housing for brewing thermostat

Postby m0n5t3r » Wed Jan 22, 2020 4:27 pm

possibly offtopic, but:
c64club wrote:
Sat Jan 18, 2020 3:50 am
Am I doing everything wrong? Didn't find any method or even a tip in user's documentation or in tutorials. What was most difficult for me:
1. Sketcher tool:
- rectangle with rounded corners had to be drawn manually, constraining fewteen things by hand, instead of just picking start and end corners.
while it's not exactly as easy as in inkscape and friends, draw a normal rectangle, pick the fillet tool and click the corners, select corner arcs and make them equal and set radius on one of them

you'll have to do this before you add other constraints, because you'll lose the corners :)
c64club wrote:
Sat Jan 18, 2020 3:50 am
- Copying "keys" shapes. They are made by cutting narrow pockets in front wall. First one (SET) Was drawn with polyline (upper half), then copied with mirror to make this symmetrical shape. I had to reconstrain everything in copied part of drawing. Second one (Minus) was done by "Create symmetric geometry" from first one. But why? Why? Why there only the lines were copied, without constrains (only few, probably randomly chosen, constrains left)? It's not a bug/lack, it's a feature, I said to myself :) I reconstrained everything one more time. With third key (Plus) I was close to to abandon the idea of making this housing on computer ("Maaaan, it takes 10x time that it's worth. Just get some plastic box laying around, cut it a bit with file and you are ready"). I found no way to just rotate copied fragment of drawing. There were two options. One was to redraw all the shape "vertically", second was to "create symmetric geometry" reflected by line of 45* angle. Both are bad and stupid, but I haven't found any reasonable alternative for them. So finally the middle key was redrawn. If I had to make 7 keys in different places and by different angles, I would turn off the computer.
no idea what you mean here; do you mean tabs like in commercial injection molded cases? those will be kinda weak when printed; anyway, it's easier to create one and then use multitransform to replicate it on the opposite walls (there's also this method demonstrated by Sliptonic: https://www.youtube.com/watch?v=BXmeEGnhszo)

as for copying the shape to make the corresponding indent pocket, try using a shape binder for the relevant face instead of copying everything, and then you can import edges / points from the shape binder as external geometry


edit: misread it, I'm not even sure why you'd overcomplicate things like that, they look easy enough to draw by hand in one go / the same sketch :) (or, if you insist, draw half of it, pocket and then mirror the pocket)
c64club wrote:
Sat Jan 18, 2020 3:50 am
-Dimensions. Every dimension had to be typed manually. Ok, I can constrain few lines with "equal" lenght then define lenght for only one of them, but I can't give them a dimension by just derive the value/size of eg. radius of existing circle.
this is a bit unclear, but: if the radius of the existing circle is set with a constraint, you can add a name for the constraint and use Constraints.<constraint name>, or <sketch name>.Constraints.<constraint name> in the expression; if the circle's radius is a result of other interactions (not set explicitly), you can draw a construction line from the center to the circle edge and make whatever lines you want equal to that; one thing that's been bugging me at times is that you can't actually add a constraint-like thing that's ignored by the solver (let's call it a measurement) that you can use in calculations later like you would with a named constraint.
c64club wrote:
Sat Jan 18, 2020 3:50 am
-If I typed some equation in "dimension" textbox, only the resulting value was saved to drawing. No way to make some rectangular hole just "2.5 times bigger than other existing dimension in project, eg than wall's height".
you can reference properties from other objects; if the wall is a pad, you can use <pad name>.Length in expressions to get the wall height; as I pointed above, named constraints can be imported from other sketches as well, and there is also the spreadsheet workbench where you can define dimensions / variables, including calculated ones, and then reference them like <sheet name>.<cell name>
c64club wrote:
Sat Jan 18, 2020 3:50 am
-didn't find a way/tool to clone some closed shape in different size
I'm not sure it's possible, indeed
c64club wrote:
Sat Jan 18, 2020 3:50 am
2. Fillets and chamfers:
-no option to chamfer/filet an internal corner, to make something similar to "corner weld".
-no option to make 1mm chamfer on egde of 1mm thick wall. Had to make 0.99mm. No option to chamfer through two pads.
yeah, these are improving slowly, but are still painful, especially at corners (I think some things even disappeared, like variable length fillets, or maybe I was using the Part workbench a few years ago, not Part Design)
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c64club
Posts: 2
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Re: 3d printed housing for brewing thermostat

Postby c64club » Wed Jan 29, 2020 1:29 am

Last week was a bit busy and I couldn't even thank you. Now we have strong wind but internet connection works. Slowly but works. Now I have time to try everyting you say. The method for taking constrains from other object resembles rather BRL CAD a bit :) more than a "clicking" CAD. But will be fun to try/learn.

In meantime I have desiigned and printed simple holders for extinguishers:
uchwyty_zdjecie.jpeg
uchwyty_zdjecie.jpeg (187.6 KiB) Viewed 845 times
Thermostats still don't run, they aren't urgent enough...
m0n5t3r
Posts: 98
Joined: Fri Feb 03, 2017 2:55 pm

Re: 3d printed housing for brewing thermostat

Postby m0n5t3r » Wed Jan 29, 2020 6:21 am

Probably the cleanest way to do parametric designs is with a spreadsheet; the second cleanest (and the one I tend to find more intuitive) is to have a master sketch (either not used anywhere and serving just as a repository for dimensions, or the way I tend to do it, the first sketch is the master sketch, edges that aren't relevant for it are drawn as construction geometry; depending on how complex the thing is, I may add side views so I can have pad dimensions defined there as well)

Granted, I have no idea what I'm doing and people who do this for a living and have to produce documentation / pass design reviews probably do it differently.