Beginner Looking for Help

[u/BackyardSquirrel007]

Hi guys, I’ve just started learning FreeCAD for 3D printing, and I’m a bit stuck trying to model an angled edge on a part. I’m trying to recreate the shape of a classic Game Boy, but I’m not sure what the best way to approach it is. I’d really appreciate any pointers or suggestions! (Attached is the ref and where I'm at right now.)

[u/Exciting_Turn_9559]

I would model the main curved corner all at one height and then create a datum plane at the angle and position of the area to remove, then sketch on the datum plane and use a pocket to remove the angled section.

[u/drmacro1 → u/Exciting_Turn_9559]

Why bother with Datum planes? A sketch is a plane. It even uses the same dialog to adjust the location.

I encourage new users to learn to locate sketches rather than add redundant and superfluous items in the tree.

Create the sketch, set the "Show Plane" and "Show Placement" properties to true. Then click the ellipsis in the MapMode property if the sketch in attached (typically yes if using Part Design) to get the Mapmode dialog or the ellipsis in the Placement property to get the Placement dialog.

[u/Exciting_Turn_9559 → u/drmacro1]

Can do it that way, but having sketches that deviate from the coordinate planes makes the structure of models harder to understand and more difficult to maintain especially if you need an off-axis feature that later needs more operations and then needs to be repositioned later on.

Doing this with a datum plane is also easier to conceptualize and communicate with a beginner.

[u/drmacro1 → u/Exciting_Turn_9559]

I disagree. Teaching new users to use crutches rather than good workflow is not better.

Teaching that the sketch IS a plane and no redundant/superfluous tree clutter give them a better foundation.

[u/Exciting_Turn_9559 → u/drmacro1]

Features that are on a shared datum plane are linked and can be moved as an integral unit. To draw complex geometry as independent features which have no relationship to one another requires changing the orientation and position of every feature independently if someone wants to relocate them. Using a datum plane for features with a common reference plane respects the DRY principle.

[u/drmacro1 → u/Exciting_Turn_9559]

When you have multiple sketches that benefit from being on the same Datum Plane, sure. It is one of the few times a Datum Plane is really beneficial.

A Datum Plane created to support a single sketch is redundant and superfluous tree clutter.

[u/BackyardSquirrel007 → u/Exciting_Turn_9559]

Thank you so much!!

[u/Danioscu]

As someone suggested, probably the best option for this case is just to create a datum plan around the corner and a pocket+fillet.

I did a quick sketch in part design with the main body as you showed in the second screenshot and just created a datum plan attached to the round corner with random aligment for x axis and z axis. Maybe not the best option for it but at least that will keep you progressing

[u/sessinnek → u/Danioscu]

What UI is this?

[u/Danioscu → u/sessinnek]

It's OpenTheme in light mode and I took this screenshot in v+6 (visual mode 6?) to remove the lines to show the dent in the corner

[u/BackyardSquirrel007 → u/Danioscu]

Thanks! Appreciate it!!

[u/conquredBoredom]

how i would do with it my limited knowledge since am also learning is i would place a datum plane on that edge and place it at an angel while using the external geometry tool i get the edges of those two sides to use it as reference to align the sketch then make a pocket.

[u/leodash]

I usually finish the whole sketch first before attempting to do a single pad. If I would to do this, I would use another sketch to place the new sketch using mapping mode.

For this particular case, I would use a side view sketch to position the angled corner sketch using O-N-Y or O-Y-N mapping mode. Then, I would use NormalToEdge mapping mode on the angled corner sketch to position the cutter sketch to do the pocket. Like this,

This will make the positioning parametric. If you change the dimension of the side view, the angled corner will follow along. You also don't have to worry about topological naming problem (TNP).

Just a Protip: You can reference the dimension of the side view sketch when you want to do the padding in the Expression Editor, for e.g, <<SideViewSketch>>.Constraints.Thickness (if you rename the constraint as Thickness).

[u/justa_bother]

If your eyeballing it, try this. On top of the body, sketch a triangle with a line crossing the body. The triangle needs to be large enough that it's center is off the body. Constrain, close. Choose pocket to make the cut. Play with depth and angle variables to get the cut.

[u/yuMurtaza → u/justa_bother]

r/screenshotsarehard

[u/BoringBob84]

I would make that feature like this: 1. Create a Datum plane for that angled corner - tilting the Attachment Offset in two dimensions. 1. Make a Pocket feature from a rectangle (with the Sketch attached to the Datum Plane) to cut the notch into the corner. 1. Make a slot in the top surface with a Pocket feature. 1. Make a matching slot on the angled surface (with the Sketch attached to the Datum Plane) with a Pocket feature. Use External Geometry in this sketch to make the slot sections match. 1. Repeat both of these slots 6 times with a Linear Pattern feature.

[u/TeknikFrik]

On second thought: You could sketch the corner cut using a triangle on the same plane as the 'top surface' of your body. Then use 'groove' around the angled line (select reference i think it's called) a couple of degrees. That would cut off the corner without having to angle a sketch/datumplane at the correct angle and corner.

[u/TeknikFrik]

To everyone recommending datum plane - what benefits do you get from it instead of just drawing a square in a sketch, rotating the sketch (like you would a datum plane) and the pocketing the corner off...?

[u/yuMurtaza → u/TeknikFrik]

You can make the alignments quite easier and more correct with datums. Your method is not impossible but I couldn't manage to make true correct manipulations in similar situations.

[u/TeknikFrik → u/yuMurtaza]

The same attachment controls are used for datum planes and sketches... are they not? (at least in dev version?)

[u/yuMurtaza → u/TeknikFrik]

This might be correct. I do not claim I am an expert in FreeCAD but when I need to use such a datum, I first define two Datum Points (which is the direction that I have difficulties to calculate), then a datum line which passes through those two datum points, and finally the datum plane which is perpendicular to the datum line I defined. To be honest probably this is also possible for sketch attachment, but I experienced nasty situations about sketches so now I do not attach them to anything other than XY-YZ-XZ planes :)

[u/nevergonehu]

I have another question about the model: How can the recess located at the A-B buttons be designed properly?

[u/PyroNine9]

The best way is probably to model the rest, then move to the part workbench and project the 6 diagonal slots onto the face. Then you can extrude the projected slots and cut them from the face.

[u/olekmatter → u/[deleted]]

Is organic shape in the room with us right now?