HR 8 wheel Bogie Tender

I was going to start this thread as a HR Barney 0-6-0 thread, but - there is always a but, I thought I'd get a bit clever - dangerous on two counts, one thinking and two assuming it may be clever

The initial batch of Barnies built by Dub & Co in 1900 were supplied with 8 wheel bogie tenders, the later batch supplied by NBL had the standard Drummond 6 wheel tenders. In addition several of the first batch had thier tenders swapped with Small Bens. So my thought was to create a model of a Barney, Small Ben, the 8 wheel tender and finally a 6 wheel tender, and I'd have several loco / tender combinations ...... simples .

As per normal, the model would be created in Fusion 360 - the free version, and 3D printed.

The locomotives are based on the drawings in Peter Tatlows Highland Locomotives.
The drawings are scanned then imported as a canvas into Fusion 360.

Now where to start - this my first loco build in Fusion 360, the HR Passenger tank was created in 123D.

I did have a few attempts at the boiler, but then thought I'd try the Tender

The drawing for the Barney has the 8 wheel bogie tender - maybe should have done the 6 wheel tender first, but that's on the Small Ben page and I haven't scanned that one yet.
A word of caution, these drawings have been drawn by hand and published at 4mm/ft (1:76), I have found that they may not be quite symmetrical.

Keeping it simple I created the floor with a couple of cutouts where the bogie pivots will be, and the buffer beam and headstock



Next up the valances

Create one, then mirror it and adjust into position



The steps have been left undersize to allow the valances to be adjusted for clearence if needed (they will be extruded to the final size).



Next the intrnal frames



And thats how it remained for a few weeks - the tender tank was a little daunting.

All these flares etc




Using the plan view I created a sketch of the main part of the tank, then created a 1mm offset towards the inside (enter -1mm into the box)





The full profile (select both inner and outer portions) was extruded to 1mm thick) then mirrored along the top edge to produce the full floor.



Aligned with the tender floor, then coppied and moved up to form the tender top.

to be continued

 

Now to create the sides.

The inner section on the sketch was selected and extruded to 1mm



Now the top edge was extruded another 1mm (to bring it flush with the top edge of the outer line).
This was then mirrored, then deleted from the lower layer to give the side profile.



Then extruded to form the sides - I'm sure someone is going to pop up and say there's a far quicker way than that - I've stumbled across it yet

Then created the wings on the front



And now the flared top

From the drawing a created a sketch of the profile




Then used the sweep command to follow the top edge of the tank



Now this is where I have now stopped, as I need to play to find out how to produce the correct profile to curve the flare down to the wings.



to follow the drawing



The brain cells need coffeeeeeeeeeeee

Paul

 

Looking at the drawings I wasn't getting how this will look, but as the saying goes a picture is worth a thousand words ........



Ah ..... thats how it looks, and note tool box, it's 90 degrees out from the drawing, looks like they moved them around as I have photos as per the drawing

so time to play .... sorry strong coffe needed first.

I made a copy of the tank body and the rim generated by the sweep command to play on.

I had to make the body a solid and change the shape at the from to get a shape that would produce and acceptable result.



Then ran the sweep command



Closer



But needs a bit more tweaking and coffee

Paul

 

ended up up spliting into several parts giving a front section that was severely fiddled and the rear section that just worked as a sweep command.



getting there - I hope

Paul

 

A little more progress below the floor, essentially buffers and vac brake assembly to go, however I think I will move above the footplate until the bogies are sorted and I have a couple of ideas for that , but you'll have to wait .

Vacuum reservoirs added, supports brackets and buffer bracing added.







Play stopped as the boss has other more important tasks for me to do

Paul

 

Hi Stan - Welcome to the dark side, most of us have started using Fusion 360 mainly the free version, there is no inference about the number of Yorkshiremen, Scots and sudo Scots in the choice of version . The choice of software was mainly due the Gauge O Guild, during the Great Lockdown of 2020, they started a 3D Special Interest Group, and a series of beginners tutorials on using Fusion 360, the rest is history.

Missing parts are a good place to start as you have a goal to aim at and should be a shortish excercise - and don't forget to post it up as we may all be able to chip in, we may even have the right answer, well we may ........

Paul

 

A little more progress

Started on the tender front and handrails - these will be brass wire.

First up the fillets at the ends of the wing plates - if anyone knows the correct name dont hold back



As can be seen I have made up the basic shape in a sketch by using boxes and a line.

These shapes were then extruded to 1mm thick. The fillet tool was used to form the curves, a neat feature is you can either type in the fillet radius, or grab hold of the arrow that appears and adjust the fillet radius until it matches the drawing.



Mirror the part and move into the correct location.

Next up the handrails

Starts with another sketch on the drawing



Easier to see without the canvas



A series of concentric circles
0.6 dia hole for the brass wire
0.9 dia for the top of the mount
1.5 dia for the base of the mount

These were then extruded and a fillet applied to produce the base



To produce the handrails - not needed for the 3D print but looks good to help visualise the model - another sketch was produced using the previous sketch for reference



Using the hole centres a rectangle was created to the side - approx 3mm.
The outer corners rounded using the fillet tool and set at 0.5mm radius
Next hide the original sketch, and delete right hand side giving ........



Finish the sketch, and apply the magic ...... well in the Create Menu select the pipe tool
Click on the blue line above for the path, the pipe will look too fat as the default diameter setting is 2mm, changs to 0.6mm and hey presto



And that's us upto date



Paul

 

Prepare to kick thy self

you need two surfaces as normal, but this tim you are making the fillet on the inner join





either enter the fillet radius, or drag the arrow



Simples

Paul