Need Advice on Modeling Tent Frame

[Sage Brush]

Hello,

First off, I'd like to say I've been tinkering with FreeCAD for a while now and am really exited. Years ago, when I started using Linux, I looked for a good 3D CAD program but never ran across anything. Yes there was Blender and others, but not something where you could site down and quickly model a bracket or drive shaft. Thanks guys!

Edit: Forgot the usual list.
OS: Linux Mint 16 Petra (Based on Ubuntu 13.10)
Word size: 64-bit
Version: 0.14.3692 (Git)
Branch: releases/FreeCAD-0-14
Hash: 5fe6e0c48f621f1136595e47cc8d7346090e7456
Python version: 2.7.5+
Qt version: 4.8.4
Coin version: 4.0.0a
SoQt version: 1.5.0
OCC version: 6.7.0

Now for my question. I'm designing a tent based on an old design known as a Draw-Tite, made by the Eureka Tent and Awning Co. back in the 1960's. The photo below is one version of the Draw-Tite. The frame consists of aluminum poles with a pin in one end that is inserted into the next pole. There are also two cross members that act as connecting hubs to hold the frame together. Looking closely, you can see two black lines running between the cross members. These are shock cords that "draw" the tent up "tite" to the frame and cause the top poles to arch.

I've worked with more simple shapes but not much with parts having 3 dimensional curves. Does anyone here have an idea on how to construct a frame like the one pictured in FreeCAD?

Thanks.

[bejant]

Hi Sage Brush, I think you may want to start with a dimensioned hand sketch of what you want to model. To create the curved portions you could create an arc to define a trajectory, and from the Part WB use the Sweep tool:

to create a solid along the arc path. I think the trick will be to orient the arc(s) correctly.

I see the two topmost tubular pieces appear to be divided into 3 sections each, the single tube over the door may be two sections, the tubes on each side of the door appear to be (two?) sections, and the rear tubes are probably sectioned too. Except for the single tube over the door I'd suggest modeling half the structure (on one side of the tent or the other side) then using the Mirror tool to make another copy.

[yorik]

Modelling this would be a pretty interesting challenge... Please share the workflow with us if you do it!

[Sage Brush]

Hi and thanks for the replies.

Well the first go around did not work so well. I tired doing most of it in the Part Design work bench so as to get a parametric model. (File is attached) I got one top pole made but as most of you know, Part Design is not the right place to do this. Each new feature can "wipe out" a feature I wanted to keep. And it seems impossible to keep going without forking the tree. The yet to be released Assembly work bench seems to be the place to do most of this.

It looks like I have two options. 1) Use the Draft work bench to draw center lines for the poles and then use the Sweep command to create the solids. In this case I will end up with a "dumb" model but that is ok. 2) I'm guessing there might be a way to make the solids and then use tools in the Draft work bench like Clone, Move, etc. to put the solids together. This hopefully would give me a model that would be somewhat parametric.

What do you guys think? If I go with the first option, I feel I will spend forever rebuilding the model for design changes. Is there a 3rd way to do this? The main problem is getting a curve in the right plane and the right length to sweep. If you look in my goofy model, you will see that the arching pole is leaning over 20* from vertical. (It's that way on the tent too.) And that I have to make the pole end in the right places so as to touch the two cross member poles (look for"cross member" in the feature tree).

-Sage Brush

[bejant]

Mostly done by eye so not exact, but it may give you some ideas:

20140814a_Tent_Frame.png (9.25 KiB) Viewed 4264 times

[Sage Brush]

Here is my second go around. Though incomplete it seems to have worked much better. I still need to mirror the side pole to the other end of the upper pole and then mirror the whole thing again. This time I used sketches to drive operations in the Part workbench with a little help from the Draft work bench. The sketches allow for some editability, which is nice. A solid is still used as a guide for the pole sketches. File is attached.

Frame 2nd Try.png (11.38 KiB) Viewed 4244 times

One thing I don't understand is why the Utility to Sweep made such garbled poles. Anyone have an idea?

bejant: Thanks! I'll have a look at the model over lunch.

-Sage Brush

[bejant]

One thing I don't understand is why the Utility to Sweep made such garbled poles. Anyone have an idea?

Try reducing the value in Edit > Preferences > Part Design (icon on left pane) > Shape View tab > Maximum deviation depending on the model bounding box. Mine is set to 0.025% and the Sweeps look OK; yours may be the default .5% - see if it helps.

[bejant]

Appearance as downloaded:

20140815a_Tent.png (18.58 KiB) Viewed 4231 times

Appearance with "Maximum deviation depending on the model bounding box" set to 0.02%:

20140815b_Tent.png (23.42 KiB) Viewed 4231 times

Pressing F5 or or the Recompute button

didn't update the model, I had to actually change the numerical value to trigger the updated view.

OS: Ubuntu 12.04.5 LTS
Word size: 32-bit
Version: 0.15.3849 (Git)
Branch: master
Hash: b64f283ce8711cd5c1f9319e937f66d8f2fcf6fb
Python version: 2.7.3
Qt version: 4.8.1
Coin version: 3.1.3
SoQt version: 1.5.0
OCC version: 6.7.0

[Sage Brush]

Hi bejant, you were right, adjusting the Maximum Deviation to 0.025% fixed the problem. Thanks.

In looking over your model I noticed that you somehow got at an angle without supporting geometry. I must be missing something, what command do you use to put a sketch in an angled plane other than mapping it to a face? Nice work by the way.

-Sage Brush

[bejant]

Thanks; to rotate the Sketch:
Without a face selected,
Select the Create Sketch tool:

Select an orientation from the pop-up menu,
Make your sketch,
Close Sketcher,
Select the Sketch from the tree view,
Click the Data tab at the lower left,
Click the three dots at the right of the Placement property:

20140815c.png (17.6 KiB) Viewed 4208 times

From the Placement window select the axis about which you wish to rotate the sketch, and change the angle to your liking:

20140815d.png (49.73 KiB) Viewed 4208 times

If you toggle "Apply incremental changes to object" to True, you can see the sketch rotate as you change the angle.

You can use the Translation portion of the window to move the sketch along an axis.

An object created from Sketches is moved by moving the very first Sketch.