I've been messing with tonight.

3D Printing
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I’ve been messing with #FreeCAD tonight.

  • I wish rotating the view had a keyboard shortcut. I don’t like middle-clicking or setting my mouse to Inventor mode.
  • I haven’t found a way to reference external geometries in a sketch yet, even though there’s a toolbar button for it.
  • While everything is indeed parametric, I don’t know how to set it up so you can set all the parameters in one place instead of digging down through to the sketches.

@Daniel_Wood , since you’re the other FreeCAD user I know about, any thoughts?

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And I’m additionally having trouble doing boolean operations! I love constrained sketching so much, and FreeCAD is on the verge of making solid modeling soooo easy.

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hello

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@Sebastian_Kuzminsky may have some suggestions.
I, too, would love to be able to work with remote parametrics. My favorite PCB layout package allows me to do much of my work via spreadsheets with all the data in tabular form. It makes stuff like placing arrays of pins trivial.

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http://www.freecadweb.org/wiki/index.php?title=Macro_Rotate_View is a macro to rotate the view plane 90 degrees. It may be amenable to hacking for arbitrary moves in cooperation with the mouse.

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I like your photo

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A 3dconnexion mouse works (sort of) with freecad witch makes rotating the objects easy . Still not sold on freecad but it has potential, parameters should be in one place I agree, but I am a freecad noob :slight_smile:

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Maybe you could join and post on the google+ freecad community…

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I’ve been using freecad to model in pure python sort of like openscad. It’s been working well for me.

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If it’s like SolidWorks, there won’t be a list of all the parameters, and you eventually won’t miss it.

Look up a technique called “skeletal modeling”. The idea is to create layout sketches that contain all the parameters you care about. You can also use these sketches to try out skeletal versions of your model before you put in the time to make more detailed models.

Another benefit of skeletal modeling is that the layout sketches are much more robust entities to make relations to. Things like vertices tend to get subtracted from the model during edits, which adds to the necessary rework.

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Nicolas has it right, join the G+ FreeCAD community or the phpbb forum where I’m always around. I’m still a total 3D printing newbie after 5 months with my printer, but I do know a thing or two about FreeCAD. :stuck_out_tongue:

To reference external geometries within a sketch, the sketch needs to be mapped to a planar face of the part you’re working on. Before creating a new sketch, click on the face on which the sketch will reside. There’s also a tool to map an existing sketch to a face. Click on the face you want to map the sketch to, then hit the “Map sketch to face” icon in the toolbar. A small dialog pops up, select your sketch in the drop down list. After clicking OK, you will be brought into sketch edit mode.

If there is no available planar face (for example you want to cut a hole into the side of a cylinder), here’s a workaround: https://plus.google.com/117324667497119008450/posts/BztXbdy94Dv

When a sketch is mapped to a solid, you don’t need to use boolean operations: a Pad will automatically be fused to the parent feature, or you can use the Pocket feature to cut away the parent shape.

When mapping sketches, you are working on a single part. When you don’t map a sketch, you are actually starting a new part, that you will have to fuse to/cut from your existing part.

The Part Design work flow is designed to drastically reduce the need for boolean operations. You still need them in some cases. Most of the time boolean failures are caused by the weakness of the underlying geometric kernel, Open Cascade, over which the FreeCAD developers have no control. But there are ways to overcome these problems, the best is to post your part so we can have a look at it.

In general when using booleans, make sure the shapes intersect; preferably they should not have coplanar faces, meaning one of the shape should intrude into the other and not sit flush. If you want to make a cut, the cutting shape should exceed from both sides of the cut part.

Finally the geometric kernel cannot deal with surface tangency. You have to remove the tangency situation beforehand. It’s a bit complicated to explain, I can provide examples if you want.

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I had no idea there was a freecad community. Awesome!

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Here’s a forum post where I explain a typical Part Design work flow, with screen captures.

https://sourceforge.net/apps/phpbb/free-cad/viewtopic.php?f=3&t=3733&start=10#p29329

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Thanks everyone! @Normand_Chamberland , I will check out the forums, and @Nicolas_Georgemel , I’ve jumped on the G+ community.

None of this was to say that FreeCAD wasn’t mostly doing what I want. I still find it easier to design parts in it over OpenSCAD, using my Solidworks background to try to guide me.

I do, however, still find it easier to design parts that are easily customized based on parameters in OpenSCAD, but that’s less of a necessity with FreeCAD because you can SEE where the parameters are on sketches, like @Dale_Dunn suggests.

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@Normand_Chamberland , I think regarding external geometry (and some other things I’ve been trying to do), I need to do some operations in a different order. Trying to work with objects that have been 3D filleted or chamferred appears to fail more often than when working with solids from the Part work bench or sketches that have simply been Padded.

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Chamfer and fillets can be tricky in most CAD programs. It is generally advised to apply them at the very end of your model, if possible.

That said, they are a little bit more problematic in FreeCAD, again because of OCC’s weaknesses. For example, pad a rectangle with a 10mm height, and try to apply a 10mm radius or chamfer to one of the top edges. It will fail. You can only get it to 9.99mm.