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Making a Start in FreeCAD

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SillyOldDuffer24/06/2019 15:46:20
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6681 forum posts
1501 photos

Part 9

So far parts have been modelled by ‘Pad’, ‘Pocket’, and ‘Loft’. This example is new - a solid made by sweeping a sketch along a path. The example is from Stewart Hart’s PottyMill Horizontal engine - I’m a fan!

Almost all parts in Stewart’s engine can be modelled with ‘Pad’ and ‘Pocket’ alone, plus a few chamfers and fillets. I’ll stick my neck out and say there’s are only two parts needing another treatment, most difficult being the rod connecting the eccentric to the valve. It is cranked to fit - highlighted in blue below:

pottymill.dwg.jpg

And Stewart’s detail drawing provides dimensions:

pottyvalvecrank.jpg

To model this, start FreeCAD as usual and open the Sketcher. As the item is 60mm long it’s convenient to turn on Grid Snap with a 10mm grid. Using the ‘Create Polyline in the sketch button’ draw a skewed horizontal line as shown, 10mm straight then diagonally down to another 30mm straight. (Remember the description of a button will be displayed if the mouse pointer hovers over it for a second or two.)

freecadpottyskewed.jpg

Before attempting to constrain the line, turn off Grid Snap. (Much confusion caused in CAD when software snaps to the wrong object, or locks something in place. Keep an eye on what snaps and constraints are on and off!)

Constrain the two horizontal lines to be horizontal with the ‘Create a Horizontal Constraint on the Selected Item’ button.

Select the two red dots on the left-hand side of the horizontal lines and click the ‘Fix the horizontal distance between two points or or line ends’ button; in the Insert Length dialogue, set Length = 30mm and press OK.

freecadpottyinserthlength.jpg

Re-select the same red dots and click the ‘Fix the vertical distance between two points or or line ends’ button; in the Insert Length dialogue, set Length = 2.5mm and press OK.

Note that in the picture I moved the dimensions to make them more readable by clicking and dragging. Double clicking a dimension allows it to be changed.

freecadpottypathdims.jpg

The sketched line defines the length and path of the PottyMill valve crank, but Pad, Pocket and Loft won’t convert it into the wanted solid. This is done by sketching a circle on one end of the path and at right angles to it. It will be swept along the line later to make a ‘pipe’, actually solid.

Close the sketcher and add a datum plane to the line. Experiment with clicking on the line; the angle of the datum plane should change. We want the plane to be at a right angles to the cranked line.

freecadpottydatumend.jpg

More...

SillyOldDuffer24/06/2019 15:46:45
Moderator
6681 forum posts
1501 photos

Part 9A

Close the datum plane tool and select the plane by clicking on it

freecadpottyselectedplane.jpg

Create a sketch and draw a 3mm diameter circle centred on the end of the path line.

freecadpottyendsketch.jpg

Close the sketcher, click on the the new circle, and click the ‘Sweep a selected sketch along a path or to other profiles’ tool.

freecadpottypipeparams.jpg

A few things to do in the ‘Pipe Parameters’ window. The Profile object is the 3mm diameter circle sketch. Corner Transition defines how bends and corners will be modelled (experiment!). Most important is selecting the Path to sweep along object. Click the ‘Object Button’ and then on the cranked line.

freecadpipeselected.jpg

The ‘Add and Remove Edge’ buttons aren’t used in this example, They allow a sketch to be piped along the edges of an object like a cube.

Clicking ‘OK’ generates the solid object.

freecadfinishedcrank.jpg

Dave

Buffer24/06/2019 15:50:41
211 forum posts
84 photos

Dave

They had a word for that, the preponderance of ths gun, obsolete now when they don't have trunions

JasonB24/06/2019 16:50:59
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19568 forum posts
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Dave, your path would be better sketched with fillets at the bends so the rod looks bent rather than mitred

bent rod.jpg

Thor24/06/2019 16:55:33
1324 forum posts
40 photos
Posted by SillyOldDuffer on 24/06/2019 15:26:07:

Very good Thor, much better than mine. Here's something to try. Because the cannon is modelled as a solid, FreeCAD knows where the Centre of Gravity is. In a real cannon the trunnions should be positioned a little forward of the centre of mass such that the gun is balanced slightly base heavy. Makes it easier to adjust elevation with a wedge or screw.

Here's how to find out in FreeCAD by adding a local coordinate system.

freecadnewcoord.jpg

Select the whole cannon then click on the 'Create a new local coordinate system' button (under mouse pointer above). Then choose 'Inertial CS' as the attachment mode. In my example the Red X and Green Y lines can be seen marking the balance point.

Try it on your cannon to see how well your trunnions are placed! Quite often if it looks right it is right.

Dave

Edited By SillyOldDuffer on 24/06/2019 15:29:20

Thank you Dave for your kind words and showing how to find the balance point. I guess I was lucky?

cannon2.jpg

I understand that adding a local coordinate system is new in v.0.18.

Thor

 

Edited By Thor on 24/06/2019 17:09:06

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