Freecad Idomatic Method for Radial Cylindrical Cutouts

[hpbmo]

I know, that fillets are sensitve. So I set the fillet radius to 4.999 mm. And if I use an expression, should it work with different dimensions

Fillet_expression.jpg (15.11 KiB) Viewed 1161 times

[papyblaise]

the radius will be limited to 4.9999mm if the precision is not enough (for the perfectionistics ), you do as in my last post:
a half horizontal piece which is higher than the XY plane, you make the radius of 5mm and a miror, the radius of 5 will be perfect

[Roland]

If someone can do without the Datum plane ...

See the solution of hpbmo
I was going to offer you another one, but it's useless, it's up to you to invent one

Hi Papyblaise,

Maybe useless, but this seems to me a very challenging modelling problem from which we can learn a lot in using Part Design WB and Part WB.

Your solution does indeed reproduce the original paper drawing. However, if I analyse your model I find a circular reference in the boolean operation that FC apparently cannot resolve:

Flange2_Papyblaise.png (55.96 KiB) Viewed 1149 times

I wonder how you were able to create it at all!

To avoid the circular loop, I propose to make a clone of the body before the boolean, turn the clone along x by 180 degrees, and fuse the two bodies. Like so:

flange2A.FCStd

(300.06 KiB) Downloaded 38 times

Best regards,

Roland, on

OS: Windows 10 Version 2009
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24276 (Git)
Build type: Release
Branch: releases/FreeCAD-0-19
Hash: a88db11e0a908f6e38f92bfc5187b13ebe470438
Python version: 3.8.6+
Qt version: 5.15.1
Coin version: 4.0.1
OCC version: 7.5.0
Locale: English/United Kingdom (en_GB)

[Shalmeneser]

If someone can do without the Datum plane ...

See the solution of hpbmo

I was asking if someone could, inside MY file, do without the Datum plane.
I need to rotate around the Z-axis by 45° (so Datum plane), then move front (enough) (so Sketch Attachment). Is it possible to do everything in the sketch Attachment ?

[papyblaise]

I don't know, it worked perfectly without a magic wand, so I couldn't answer

[Shalmeneser]

...

Your first pad is "2 lengths : 10 & 1" ???

Code: Select all

OS: Windows 10 (10.0)
Word size of FreeCAD: 64-bit
Version: 0.20.25311 (Git)
Build type: Release
Branch: master
Hash: c5524bb58a7126fa2242d6137eb82ee9d54e82d4
Python version: 3.8.10
Qt version: 5.12.9
Coin version: 4.0.0
OCC version: 7.5.2
Locale: French/France (fr_FR)

[chrisb]

I know, that fillets are sensitve. So I set the fillet radius to 4.999 mm.

Sorry, I had set my precision to 2 decimals and didn't see the two lines. I was already slighty delighted, that OCC had improved the fillets.

[chrisb]

Maybe useless, but this seems to me a very challenging modelling problem from which we can learn a lot in using Part Design WB and Part WB.

It is indeed interesting and I still don't fully understand why the PartDesign Pattern needs the sketch to have an offset. Even manual setting of the Overlap property didn't help.

[papyblaise]

Your first pad is "2 lengths : 10 & 1" ???

as I said, to be 1mm above XY to have enough material to make an R = 5

I need to rotate around the Z-axis by 45° (so Datum plane)

he ben alors you don't how do that ...
you who give the impression of taking everyone back to do better
you just have to draw it on the XZ plane and turn it on its Z by 45 °
you just have to know that its Z is the Y of the general reference
each time you change the local plane, the Z of the sketch is perpendicular to the screen, which is not the same as in the general
it is thus in all the CAD that I know (tous les CAD le sont french jok)
green : mine , white : yours , you can see it's same result

[chrisb]

Is it possible to do everything in the sketch Attachment ?

Sort of:
- Attach the sketch with Mode FrenetTB to the 60° arc of Sketch
- To get 45° of these 60° we use the MapPath parameter with the factor 45/60 = 3/4
- Add an offset to z direction of 10mm
- Reverse the pocket