3D cad; drawing a locomotive wheel

[sis]

Hi,

I am very much a raw beginner with 3D cad. I am currently trying to use Fusion 360, primarily because I can afford the price!

I've made some progress drawing simple objects like the frames, assemblies for stretches, drag boxes etc. I am hoping to improve my skills by tackling drawing a locomotive wheel and eventually a cylinder. I have works drawings to follow complete with side and face projections and sections.

There was a recent and very educational thread about drawing a safety valve. Several posting with solutions of how to do it. I am wondering if a kind soul could explain their approach for drawing a wheel? I don't mind if it is with an alternative cad program as I can research the equivalents in Fusion360 and give it a try. All help appreciated.

Thanks,
Steve

[Roger]

Hi Steve,
I assume that you can create the hub and rim easily enough, it's the spokes that present more of a problem. I've never tried to model an accurate wheel, but this is that I'd do....

1) You're probably only going to model one spoke and then create all of the others from it.
2) The spoke will probably change in section, but you can't really use a simple extrusion with a taper on it, because you probably want to keep the back of the spoke flat.
3) I'd draw the start and end cross sections, creating two planes one near the centre and one somewhere in the rim where it will be covered by the rim when you model that.
4) Once you have the two sketches, you should be able to use a Loft or similar to create a solid with those two sketches as the ends.
5) Model the inner and outer rims
6) Create a circular pattern of the single spoke.
7) Add fillets. This can be troublesome, you'll soon find it complains for no reason sometimes.

I'm sure there are many approaches, but that would be my first port of call.

[sis]

Hi,

Thanks Roger. I apologise for not replying sooner. I was caught out by a busy week at work and the family threw up a few extras as well.

I'll be looking at playing with the loft feature in the next few days.

Thanks,
Steve

[sis]

Hi,

This is where I am having difficulty In drawing a spoke. The wheel is a GWR 3' 2" Bogie Wheel. I have selected this wheel to draw as a learning example as I have a good works drawings (No. 89997) from Didcot and it is about as simple as it gets. My actual immediate plan was to draw up 9F wheels but I have photos that are not quite good enough to make out a fair few of the dimensions. So whilst I work on solving that I need to keep learning with the Fusion 360. Well hopefully an image will appear:




I apologise for my terminology. I expect it is incorrect but I hope it will be sufficiently accurate to communicate. Please feel free to educate me on better terminology.

I have drawn the hub and the rim (minus the tyre). On the works drawings there are 2 side view cross sections for a spoke. I have the side view of a spoke and a top view. I have made sketches for each of these. When I use the loft command with the 2 cross section I am able to loft and get a reasonable partial spoke. However the bit I am stuck on is how to incorporate the top view and side view sketches to allow that loft to continue in to the rim and into the hub. I have tried projecting the sketch of the cross section on to the rim and of course that does not take in to account the top and side view sketches.

Any and all advise appreciated.


Thanks,
Steve

[Roger]

Hi Steve,
There are probably two ways to approach this.
In my opinion you need to define the two end sections whatever solution you end up with.
You can then either create several more cross sections among the length to guide it, or use guide curves to do that.
The first is much less troublesome from the point of view of software complaining.
Guide curves do work but they have to intersect every cross section in the right order and at the precise point, say a corner, on each one. Unless it's perfectly right, it just won't work, and it won't tell you why in a way that makes sense.
So you can use the side view to create the guide curves from that. On my CAD system, you have to draw the guide curves as 3d sketches, and that's very clumsy. Hopefully it's easier on Fusion360

[sis]

Hi Roger,

I had a play for another hour or so last night. I started to create a series of additional spoke cross section sketches which includes the ends; although since the works drawings do not have said cross sections I am in effect making it up as I go along. I had hoped perhaps naively that the clever software would be as clever as the pattern maker and be able to finish the job with just the information on the drawing, in hind sight I see that it couldn't without more cross sections. I'll be doing some youtube fusion360 video watching on loft and guide curves before I work more on it.


Thanks,
Steve

[Roger]

Hi Steve,
Do have a play with guide curves too, they will steer the path that the geometry takes between the end sections. If one side of the spoke is flat, you can probably create a curve that follows the edge, but whether you can make it accept that is another thing entirely. My experience is that the more complex the geometry, the less likely it is to accept guide curves without complaining.
It might be possible to do it that way with only the end sections though. All you can do is experiment and see what you can get to work. What I'm pretty confident about is that with multiple cross sections and no guide curves, you will almost certainly get it to create the 3D shape. You may find that you need quite a few sections though to get a smooth transition from end to end if there are significant changes in section.

[nick952]

Hi Steve,

If I understand the question correctly you want to extend the length of the spoke, in proportion to the cross sections you have.

In Alibre Design, after the Loft using the two cross sections you have from the drawing, using the "Move Face" Direct Editing tool does what you need. In this case moving the selected faces and maintaining the tapering form proportions (the origional loft size/form remains unaffected).

A quick test:-

Initial loft.


First face moved.


Second face moved.


Notice the original Loft Sketches are still showing in red and are unchanged after the face moves.


Do you have a similar Tool/Command in Fusion?

After lengthening the spoke (slightly longer than needed), you'll either need to use other commands to trim the ends to length, with the correct form, or possibly after creating a circular pattern of this larger spoke, use a Boolean unite and then fillet each spoke, hub, rim intersection.

Hope this helps.

Nick.

[jools]

Hi Steve,

I was browsing some of the you tube tutorials for Fusion 360 out of interest today and finally see how powerful it can be, also the videos of the CAM aspects of it.

I did come across this basic spoked wheel tutorial whcih you may have already seen, but perhaps there is some clue in it that will help.....

www.youtube.com/watch?v=uQTNBC_ldhs

regards

Jools

[sis]

Hi,

Thanks to all for the replies. All the responses have helped. To clarify the main issue was using "loft" to model a spoke i.e. getting the software to do what you wanted it to. I settled on the following method which had some iterative steps with adding additional cross section sketches as required.

1. drew a sketch in the plane of the center of the spoke with lines at 90deg for each cross section. I then created an offset plane referenced to these lines to sketch the spoke cross sections on.
2. Sketched the cross sections that the drawing supplied.
3. Added additional cross sections as required. All referenced to lines and offset planes from the sketch in 1.
4. 1 Loft between the known cross sections.
5. 2 additional Loft, 1 each from the known cross section out to either the hub or rim. I had to play about with additional cross section sketches to get the software to do what I wanted.

I found if I tried to loft the whole spoke in one go the software did not get it right. I wasted a lot of time with trying to get it to do that and the breakthrough was to realise it didn't matter. Split the loft job up into 3 sections. hub end, middle section, spoke end.

Once I based the solution around the sketch in step 1 I could then play about with lofting and based on the results adding cross sections in a planned way and redoing the loft until I got the software to do what I wanted.

I am sure I have lots to learn about loft still. I now have more understanding, and empathy when Roger comments about "fighting the software".


My next step will be to research guide curves to see if I can reduce the amount of cross sections I need to "invent" and try and have more reliance on the cross sections and plan and side profiles that the drawing details rather than lots of cross sections I make up to make it "look" right.

I also have a lot more respect for the efforts that people have put in to model this type of component. I can see that a prototypical driving or coupled wheel is a lot of work, and a cylinder from works drawings is a massive amount of work.

Thanks,

Steve

[sis]

Nov 17, 2017 11:22:23 GMT nick952 said:

Hi Steve,

If I understand the question correctly you want to extend the length of the spoke, in proportion to the cross sections you have.

In Alibre Design, after the Loft using the two cross sections you have from the drawing, using the "Move Face" Direct Editing tool does what you need. In this case moving the selected faces and maintaining the tapering form proportions (the origional loft size/form remains unaffected).

A quick test:-

Initial loft.


First face moved.


Second face moved.


Notice the original Loft Sketches are still showing in red and are unchanged after the face moves.


Do you have a similar Tool/Command in Fusion?

After lengthening the spoke (slightly longer than needed), you'll either need to use other commands to trim the ends to length, with the correct form, or possibly after creating a circular pattern of this larger spoke, use a Boolean unite and then fillet each spoke, hub, rim intersection.

Hope this helps.

Nick.

Nick,

Thanks. I'll research these terms and functions in Fusion 360. Lots to learn......

Thanks,
Steve

[sis]

Nov 18, 2017 6:53:37 GMT jools said:

Hi Steve,

I was browsing some of the youtube tutorials for Fusion 360 out of interest today and finally see how powerful it can be, also the videos of the CAM aspects of it.

I did come across this basic spoked wheel tutorial whcih you may have already seen, but perhaps there is some clue in it that will help.....

www.youtube.com/watch?v=uQTNBC_ldhs

regards

Jools

Jools,

Thanks. I think the issue boils down to selecting the correct approaches to draw the spoke in the most sensible way with the information on the works drawing. There is not sufficient information to simply loft between cross sections as there are insufficient cross sections. When I get some quite time tonight I'll be watching videos on guide curves.

One of the nice things about the 3D cad is that I am working on it in the lounge. So it doesn't count as workshop time! :-)

Thanks,
Steve

[jools]

Nov 18, 2017 11:29:08 GMT sis said:

Nov 18, 2017 6:53:37 GMT jools said:

Hi Steve,

I was browsing some of the youtube tutorials for Fusion 360 out of interest today and finally see how powerful it can be, also the videos of the CAM aspects of it.

I did come across this basic spoked wheel tutorial whcih you may have already seen, but perhaps there is some clue in it that will help.....

www.youtube.com/watch?v=uQTNBC_ldhs

regards

Jools

Jools,

Thanks. I think the issue boils down to selecting the correct approaches to draw the spoke in the most sensible way with the information on the works drawing. There is not sufficient information to simply loft between cross sections as there are insufficient cross sections. When I get some quite time tonight I'll be watching videos on guide curves.

One of the nice things about the 3D cad is that I am working on it in the lounge. So it doesn't count as workshop time! :-)

Thanks,
Steve

Steve,
I started to understand the loft process through the Lars Christensen tutorials which, as a total 3D CAD virgin , not currently having Fusion loaded and coming from a 2D CAD background (albeit it AutoCAD so basic commands are intuitive) I found excellent. He also covered the loft process from using a background sketch to create the cross sections and showing the process including the guide lines, so going back and reading your initial posts started to make more sense.
I also stumbled across another very good tutorial which covered the Sculpting process, which I also found fascinating. Not sure that this lends itself to a more symmetrical model though.

I'm glad you are working through this and look forward with eager anticipation to the final result.

Jools

[jools]

BTW,
the SMEE website does have Fusion360 online workshops and videos, if you are a member, which although lengthy do take you through some of the processes and problems encountered by the members and it does seem that filleting models can be problematic with many different causes - a couple being stray lines that interfere with the the constraints during filleting, and loss of references if copying across.

One video actually goes into drawing a locomotive 12 spoke wheel, but unfortunately gets bogged down due to some of the problems I mention above.

Jools

[Roger]

It's worth commenting that filleting anything other than simple geometric shapes can be very troublesome. This is true of any 3D modelling package. Sometimes you can happily add fillets to one side of a symmetrical shape without difficulty, only to find that it just won't play when you do precisely the same on the other side!

It can be a deeply frustrating process, experimenting with different filleting radii and changing the order they're done with. Sometimes it simply isn't possible and you have to think of another way to model the feature.

[joanlluch]

Nov 19, 2017 12:54:49 GMT Roger said:

It's worth commenting that filleting anything other than simple geometric shapes can be very troublesome. This is true of any 3D modelling package. Sometimes you can happily add fillets to one side of a symmetrical shape without difficulty, only to find that it just won't play when you do precisely the same on the other side!

It can be a deeply frustrating process, experimenting with different filleting radii and changing the order they're done with. Sometimes it simply isn't possible and you have to think of another way to model the feature.

To my experience it’s a matter of which order you apply fillets to corners. If the final geometry with all the fillets applied has some sense at all, then the filleting is always possible. If this is troublesome for some cases, I can only guess that different CADs may have different internal algorithms at creating fillets, and not all of them will fail on the same scenario.