Irregular linear array... a better way?

[cleahcim]

top-yaw.FCStd

p2

(268.09 KiB) Downloaded 46 times

I'm trying to Create a irregular linear array of arches on a plane. I finally got it to work, but I'm sure there is a better way. In ascii art I'm looking to create two parts that mate:
p1.) 0_0__0_0 //

top-yaw.FCStd

p2

(268.09 KiB) Downloaded 46 times

I
p2.) 0_0_00_0_0 //

yaw2.FCStd

p1

(80.79 KiB) Downloaded 39 times

then, place a through pocket in all the arches making a hinge.

P1 would flip over 180 degrees and the double __ would mate with the double 00 of p2. I've attached what I've done, but I would love to hear some feedback on an easier/more-flexible approach. It is a lot of work if I decide to make some changes on these two parts.

For the 'yaw2' part (eg p1) I went with a multiple transform. I had to keep the arch part nested in the base or it would disappear. These seemed adequate, but I think I should be able to draw/pad a rectangle base, put a draft line of where I want the array to start, and then execute the ray and union the pieces. I couldn't figure it out though. The current method makes it hard for me to adjust my tolerances for printing.

The top-yaw (p2) part I was trying to start with a middle out approach and do a linear array out. I failed at that, I became desperate to finish the part and didn't the worst way I could think of doing it... I just kept adding sketches and pads until it was done.

Any guidance on how to do this better, let me know. I like the power of Freecad, but the usability has a ways to go.

The end goal is a simpler way to do this:


OS: Windows
Word size: 64-bit
Version: 0.14.3700 (Git)
Branch: releases/FreeCAD-0-14
Hash: 32f5aae0a64333ec8d5d160dbc46e690510c8fe1
Python version: 2.7.6
Qt version: 4.8.5
Coin version: 4.0.0a
SoQt version: 1.6.0a
OCC version: 6.6.0

[DeepSOIC]

My suggestion would be to create a simple linear array on both parts, and then eat away the excess ones with a single pocket.
EDIT: Looked at the model... looks like my suggestion is a bit stupid...
EDIT2:And welcome to the forum!!

[jmh]

Welcome to the forum.

I'm not sure I have much of a suggestion on the array -- other than may trying to create the regular spaced object and then remirror that with a different spacing. My question on that is "Is it necessary?" -- if you are making both parts maybe just let them be symetric, I would think the hing will still work.

The other thing I'd suggest that will make the effort much easier is to remember FreeCAD is a solid modeler. You can apply cuts and joins (booleans) to bigger solids to get what you want. Maybe a disk, a bar and an arch as the three base solids. Cut the center hole in the disk, bolt holes with polar mirror. Drill a hole through the arch and then apply cuts for the hinges to mate up. Seemed like you were building up from some small solides and then fusing more pieces together.

I suspect others will have better suggestions as I'm still pretty new at this as well.

John

[NormandC]

Hello cleahcim,

Welcome here.

I'm struggling to understand how you made your top-yaw model, unfortunately I don't have much time left tonight.

What puzzles me is your use of Part Refine features. Why create a refine of a refine? Moreover, Pad006 which was refined into refine_Pad006 didn't even need a refine to begin with.

Fusion is a boolean union of objects sharing a lot of coplanar and tangent faces. This is usually bad practice because it can lead to geometry errors.

Then there's the "Fusion001" object which has no starting point. Its icon indicates it's either a simple copy or a shape made from the "Part --> Refine shape" menu. This object is non-editable.

Hopefully other will join in with their suggestion, if not I'll come back tomorrow with suggestions.

[NormandC]

Hey what do you know... Couldn't resist. Sleep is overrated.

Here's my take on top-yaw. Same basic idea than jmh suggested, starting from a solid hinge and cutting slots in it - but doing just half of it longitudinally, then mirroring the body with Part Mirror, and fusing the original and the mirrored copy.

I didn't bother making the holes on the washer. I noticed yours in Sketch009 were partly covered by the back plate of the hinge. This is why it's best making a new sketch and applying a Pocket.

One thing I'm not too happy with is how the cuts left the perimeter edges in segments, which showed when I applied fillets on them. (this is due to a bug in OCC, the geometric modeling kernel used by FreeCAD - the refine shape tool in the Part WB and the refine shape feature in the OpenSCAD WB try to address that)

Be advised I modeled this with the current development snapshot of FreeCAD in which the OpenSCAD Part Refine feature benefited from a recent upgrade. So if you attempt to edit this model with the regular stable release, you might get unexpected results.

I'll be happy to answer any questions you might have on my modeling method tomorrow.

P.S. I'm not too sure I followed your original dimensions exactly.

[NormandC]

Duh. Should have made the first pad twice longer, then created a Part Design Mirrored feature rather than a Part Mirror. The fusion wouldn't have been needed.

Oh well.

[cleahcim]

You did in less than an hour in a much more elegant way what took me forever to do. I guess I was too focused on the array approach vs the modeling aspect of it; adding to the feature what I want instead of taking away to get where I want to be. I could of reached out earlier to save myself a lot of brain ache.

The refine of the refine (repeat) is a setting I have in FreeCad to always refine after an addition to a part. It helped me in the beginning but I probably should flip that setting off.

I'd like to model the henge/arch piece(s) idependently of the rectangular base and position it in an ad hoc manner on the rectangular base. I failed to see an action that would allow me to select a face and position it on another face. Does that exist in freecad?

[jmaustpc]

I'd like to model the henge/arch piece(s) idependently of the rectangular base and position it in an ad hoc manner on the rectangular base. I failed to see an action that would allow me to select a face and position it on another face. Does that exist in freecad?

Edit menu ... Alignment ..... select three points on each of two solids and they will be aligned.
Draft WB Move...in conjunction with various Draft snapping, turn on only the snap type/s you need.
or just edit the placement parameters
or use Edit menu Placement tool which can also be used in either absolute or relative modes.

Assembly in your version of FreeCAD is completely non functional ...actually pretty much non existent. However it will do the above functions but with definable constraints that auto update, when Assembly is one day added to master.