Element repeated multiple times at an angle?

[kefir]

Hi,

I'm struggling with a design, and I wonder if I'm not understanding how I'm supposed to design something like this. I'll try to illustrate, here's an incomplete version of a design:

Screenshot from 2019-01-20 21-46-19.png (158.63 KiB) Viewed 1652 times

So, I have a fairly simple base shape that is almost an isosceles trapezoid, extruded to a fairly thin solid. The longer parallel edge is furthest away, the shortest parallel edge is nearest us.

On the far side there's a "tube" or tunnel, which is basically for a hinge. On the near, slimmer end of the base shape, I want 4 or 5 "tubes" - but with some additional details. There's an additional copy of these parts to the right in the screenshot. They are pointing towards us but their rotation should be evenly distributed from left to right. The ones along the edges are parallel to the edges, but the ones in the middle won't be. I guess they should roughly be pointing towards the same point in the distance, but I'm really not that concerned about this. An approximation is fine.

How would you go about designing this? I think I'm simply doing this wrong.

I figured I'd use the assembly2 workbench a try for this, so I designed some basic shapes and proceeded to assemble them as I needed. I gave up assembly2 just before chewing my screen with frustration. I moved on to a2plus, and I've managed the hinge at the back, and the two along the sides. I'm not sure how to place the 2-3 final tubes between these, with the rotation. And even if it's possible using assembly2/a2plus - what is the "correct way" of drawing something like this in FreeCAD?

I've included the freecad files of the basic shapes. They were made in FreeCAD 0.17 from the stable ppa, I'm currently running a FreeCAD 0.18 AppImage downloaded today. I installed a2plus using the addon manager. I was using an older version of assembly2, and after I tried upgrading it started crashing immediately when I added any part to an assembly. I'm on Ubuntu 18.04.

[NormandC]

Hi,

What's exactly your intent? I see multiple bodies in your screenshot, but isn't this intended to be a single part?

[chrisb]

You can use Draft->Array on polar mode. The center is the point in the far distance where the prolonged lines of the sides would cross.

[kefir]

Hi,

What's exactly your intent? I see multiple bodies in your screenshot, but isn't this intended to be a single part?

Yep, I want 2-3 copies of the little part on the right side to be evenly distributed and rotated between the two I already attached.

[kefir]

chrisb's suggestion for draft polar array worked nicely, actually. So I've used a2plus to import the element and place one where it should be, and finally rotate and distribute from there. I think I get stuck trying to solve problems in a single workbench for some reason - I'm not new to FC, but I've mostly dabbled with part design. Here's the result:

Screenshot from 2019-01-20 23-52-56.png (179.92 KiB) Viewed 1628 times

Of course, it'd be nice to be able to snap the first and last element to some edges/planes/etc, and get the polar array to fill in the remaining number for a perfect fit. Or is this also possible in FreeCAD already? I just winged it, I experimented a bit with some values for center point and the angles of rotation, and I managed to get a fit that's close enough for practical purposes.

Thanks for the help.

[NormandC]

Yep, I want 2-3 copies of the little part on the right side to be evenly distributed and rotated between the two I already attached.

You did not answer me. Do you intend for the hinge and the pin holders to be fused, unioned to the main body? It seems only logical to me. So there is no logical reason to model them in separate bodies. This could be all modelled in a single Body. No need for an assembly add-on.

Assemblies are for joining parts or bodies that will be manufactured separately, then assembled together by gluing/bolting/welding/etc. If what you are modelling is to be a single part, you don't need assembly.

Meanwhile you posted another reply that just seems to prove to me that you are doing it wrong using an Assembly add-on.

What's next with this? Once completed, what are you going to do with this model?

[NormandC]

Please have a look at this model. Everything was modelled in a single FreeCAD document, and in a single PartDesign Body. Unless I'm completely mistaken, that's what you are actually after.

FC_kefir_main_plate_01.png (57.61 KiB) Viewed 1624 times

The datum plane is used to attach the sketch to create the Pin_holder. The datum plane was created from one edge of the Base_plate sketch, with attachment mode set to "normal to edge". Attaching to a sketch is a little more robust than attaching to a 3D feature.

In most of the sketches, external geometry is linked to other sketches rather than to edges on the Body, for the same reason. When working in a sketch, I simply hide the 3D feature and show the sketch from which I want to link external geometry.

The DatumLine_Pattern_Axis is used for the PolarPattern axis. Its location is controlled by a reference dimension named DistAxis in Sketch001 (under Base_plate). The PolarPattern includes Pin_holder, Pin_stopper and Pin_guide. The angle of the Polar pattern is also set with an expression linked to a reference dimension in Sketch001, named Angle. In this way, everything is linked to the angled sides on the base plate. For example, edit Sketch001 and change the 24mm horizontal distance constraint to another value, and everything will update.

Let me know if you have questions!

Normand

[kefir]

Thanks Normand, this looks like it's exactly the kind of stuff I need to understand, which I currently don't. As a novice modeller, it's not always easy to get how the software developers intend for the tool to be used for different tasks.

[kefir]

Normand, I'm trying to work my way through what you've done, picking up some nice tricks on the way. But when I recreate a simpler version (attached), I get some different numbers. My center of rotation, auto-calculated by attaching a point to where the two lines would meet in the distance, is different from yours, even though I'm trying to recreate the sketch with the same measurements. I get 215, you got 177,417. The angle looks the same, though. But as a result, when I try to rotate by the angle, it doesn't align nicely like yours.

Would appreciate any input.

[kefir]

Hmm, looks like I suddenly managed. This time I snapped the point for Center of Rotation to a reference line 2.5mm to the right of the actual edge, like I realized you probably did. To match the center of the parts to move/rotate? Now I get 177.5, while you got 177.417 or something very close. My angles were still off, but my DatumLine didn't reference Z_Axis, i selected the top face and chose the principal axis that looked like Z. I don't get why this shifts my result slightly - maybe it's centered in the object instead of (0, 0)?

Thanks for the help! Not sure I understand all the details, but at least I've managed to recreate the basics of what you did.