Struggling with workflow on a chassis design

[Anonymous]

I'm attempting to design a tube chassis for a race car and I don't think I'm using proper workflow. I've gone through the beginner courses, watched YouTube videos, and read every thread I can find here on workflow related to automotive designs. The design is complex and involves over 300 tubes of different diameter and thickness. I'd like to be able to edit each tube individually and have the sketches change with the tubes if/when I need to edit them. I'm not really sure where to start; Should I create a complete wire frame of the chassis first and then use the "pipe" feature to create each tube as a new component? Should I start with an empty component and then create a sketch within it for each tube and then use the "pipe" feature to create each tube as a body? Does every sketch need to be constrained before I attempt to create a body/component from it? I'm beginning to think I may be overthinking it a bit but I'd really like to do it the right way.

I appreciate any suggestions, screencasts, and links to anything similar if anyone can provide them.

Thank you all for any help.

[chrisplyler]

Personally, I would use sketch(es) at the top level to create a wire frame representation. At miter joints, you'll want to extend the lines and add a short line representing the miter angle.

Then I would make a new component and pipe one line. Make another new component and pipe the next line. Etc. Etc. Etc. until I had the whole thing piped.

Then I would go back and split body using those miter representation lines. Remove the extra bodies this creates.

Combine/cut/keep pipes that need to be drilled so their ends fit around other pipes. Remove any extra bodies this creates.

[kb9ydn]

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@Anonymous wrote:

I'm attempting to design a tube chassis for a race car and I don't think I'm using proper workflow. I've gone through the beginner courses, watched YouTube videos, and read every thread I can find here on workflow related to automotive designs. The design is complex and involves over 300 tubes of different diameter and thickness. I'd like to be able to edit each tube individually and have the sketches change with the tubes if/when I need to edit them. I'm not really sure where to start; Should I create a complete wire frame of the chassis first and then use the "pipe" feature to create each tube as a new component? Should I start with an empty component and then create a sketch within it for each tube and then use the "pipe" feature to create each tube as a body? Does every sketch need to be constrained before I attempt to create a body/component from it? I'm beginning to think I may be overthinking it a bit but I'd really like to do it the right way.

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The chassis has 300 separate pieces?  That seems like an awful lot for just a chassis unless that includes the suspension as well.  And even then it still sounds like a lot.  With that many pieces you won't want to make a component for every piece; that will be a mess to manage.  I would try to break up the chassis into some sort of logical groups and then use a single component for each group.  Within each group you have the individual tubes as bodies.  This way you can work on a single group at a time and hide the rest so it's not so visually overwhelming.

The wireframe and pipe method will probably be the easiest for modelling, as opposed to wireframe + sweeps.  If this is something that will be welded up from actual tubing you will need to think about how to lay out the joints so that the whole thing can be assembled.  You wouldn't want to get halfway through fabrication and find out you can't physically fit some of the tubes where they need to go.  With the number of tubes you're talking about this could be a significant challenge.

As for creating the wire frame, I don't really have any suggestions there.  Unfortunately Fusion is not very good for sketching 3D wire frames and it's hard to offer specific suggestions without seeing the actual design.  I suspect you're going to want to make heavy use of construction geometry for defining the positions of drive train components and such.

As a general rule it is always a good idea to fully define sketches before using them to create bodies, even if you just assign temporary dimensions that you know will change later.  I also like to use geometry relationships as much as possible, as opposed to numerical dimensions.

C|

[Anonymous]

These are some screenshots from a incomplete and rough model I made in Shapr3D to give you a better idea of what I'm trying to create in Fusion 360.  

So far, I haven't been able to make a decent wire frame due to my inexperience with 3D sketching in Fusion and in general. I appreciate your advice and I have been trying to break the chassis down into sections. I've started on the floor of the chassis but haven't been able to get past the rocker bars because the front crossmember is supposed to kick up a little on the ends and I haven't found a way to make the seat support and floor triangulation bar move along with it. Hopefully that works because this has been quite a fight. 

Thank you for your input and I would appreciate any more advice you or anyone else can give me.

[davebYYPCU]

There doesn't appear to be many pipes that don't lie on a plane.  I would be doing one side, mirror and then join across

most of the sections would be 2d sketches.

Might help....

[Anonymous]

Thank you for your advice. I haven't tried creating side planes to start with and then connecting them, but I will. 

Some of the problems I've run into with the sketch are difficult to see with the pictures I provided. For example; The floor would need two planes, both on different angles. 

The main frame rails (bottom inner tubes) are sloping upward from left to right in this picture, while the rocker bars (bottom outer tubes) are sloping downward from left to right. The rear crossmember is in line with the main frame rails while the rocker bars do not because the front crossmember tubes kick up for exhaust clearance. It's a very small detail and hard to see and explain but it's also very important. 

front viewRight side view (front is on the left, rear is on the right)rear view, at a slight angleHopefully these screenshots give some insight into the problems I've been running into with the floor. I'll try to figure out how to lay out construction lines and project planes through them to give me the surfaces I'll need to sketch these out in 2D. I just need all of the tubes to be connected when I'm finished and I'm trying to figure out how I can make all of the points meet where I need them to if I'm using two or three separate planes and they are separate 2D sketches. It seems I would need to connect all of the points in 3D, but if I can get the planes to intersect exactly where I need them to I could see how it would work. 

Thank you again, I'd still appreciate any input. 

[davebYYPCU]

Doesn't look like a free hand design, so there will be enough datum points available. 

Planes can be made in a lot of ways, Offset, on Angle, on Path, and 3 point, so it's picking which one.

Eg: The centre line of each pipe has an infinite number of planes at Angle.

Can you share the file?

[chrisplyler]

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@kb9ydn wrote:

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The chassis has 300 separate pieces?  That seems like an awful lot for just a chassis unless that includes the suspension as well.  And even then it still sounds like a lot.  With that many pieces you won't want to make a component for every piece; that will be a mess to manage.  I would try to break up the chassis into some sort of logical groups and then use a single component for each group.  Within each group you have the individual tubes as bodies.  This way you can work on a single group at a time and hide the rest so it's not so visually overwhelming.

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You've got the right idea, but the wrong implementation.

He should decide on groups and then make a Component for each group. Then he should make SUB-Components within those groups as appropriate. For something like a tube frame chassis (and really most stuff) you want each individual cut pipe to be a Component. If you have them as multiple Bodies inside a Component, you're really limiting yourself.

[chrisplyler]

In the pictures you provided, it appears that the design as predominantly planar. Sure, you will need several different planes, but that's no biggie.

I would start with the floor plane. Sketch all the lines on it that ARE planar. Center one of the symmetrical cross bits on the Origin, and sketch the rest of it relative to that.

Then, where stuff needs to start angling up, pick one of those lines you've already sketched, put a plane-on-an-angle on it, and start sketching the appropriate stuff.

Start with the flat floor stuff. Then work up around one side. Then mirror that side stuff. Then connect the sides together where you haven't already.

[chrisplyler]

In fact, the planes are a good way to group it.

Make a Component for each planar set of pipes. Make the plane you need within that Component. Make the sketch within that Component. Then make a new sub-Component for each pipe.

When you have a Component with sub-Components inside of it, you will notice that the "container" Component icon turns into an Assembly icon.

When you start welding, it makes sense that you will probably weld up planar sets together first, as that suits clamping stuff to a welding table, right? So it's kind of logical to organize things this way.

You might do something like this:

Overall Assembly

>Front Clip

>>Flat Floor Members

>>>Pipe 1

>>>Pipe 2

>>>Pipe 3

>>Angled Floor Members, Left

>>>Pipe 4

>>>Pipe 5

>>Side Members, Left

>>>Pipe 7

>>>Pipe 8

>>>Pipe 9

>>>Pipe 10

>>Front Cross Members

>>>Pipe 11

>>>Pipe 12

>>Top Cross Members

>>>Pipe 13

>>>Pipe 14

>Cabin

>Rear Clip

You would Mirror Component for Angled Floor Members, Left and Side Members, Left, and then rename the mirrors as Angled Floor Members, Right and Side Members, Right.

Make sense? Do the same sort of stuff for the Cabin and the Rear Clip.

[kb9ydn]

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@chrisplyler wrote:

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He should decide on groups and then make a Component for each group. Then he should make SUB-Components within those groups as appropriate. For something like a tube frame chassis (and really most stuff) you want each individual cut pipe to be a Component. If you have them as multiple Bodies inside a Component, you're really limiting yourself.

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Most of the time I follow the one body per component rule pretty strictly.  But for things like weldments where the final product will be a solid contiguous structure, it makes more conceptual sense (to me) to treat the whole structure as a single component.  But it also depends on how you want to model the structure.  If you intend to use joints to connect all of the pieces together, then for sure you want to have each piece be its own component.  But if you're going to start with a 3D wire frame "sketch" and then apply the pipe command to the wires; having every individual piece be its own component gains you nothing.  It really just adds complexity for no reason.  Yes, multiple bodies in a component is more limiting (e.g can't use joints) but that's the whole point.  Every option that you don't have available is one thing that you don't have to manage or keep track of.  The tricky part is knowing when to limit your options and when to not.

I'm not going to say that there is a right or wrong way to do this, there really isn't.  This is very much getting into style and preference; what makes the most sense to you and how are you most comfortable doing things?  I used to think multi-body modelling was totally weird and didn't really understand why you would ever want to do it.  But then I discovered that in some cases it's actually easier than assembling individually modeled pieces.  So now I use it more often.

One other thing I was going to say (this is more about the design than modelling technique) is that it looks like a fair number of the tubes could be consolidated into single pieces.  I'm no expert in tube chassis design but some pieces look like overkill and others look like they could be a single piece with two or three bends.  It's a balancing act of course with how many bends you can put in a single piece.  More than 3-4 bends in a single piece is likely going to be difficult to make with high accuracy unless you have a CNC tuning bender.

C|

[Anonymous]

This makes a ton of sense and is actually how I've had the most success so far. I seem to have trouble with getting the mirror feature to cooperate but I'm sure it's just something I'm not doing right, and I'll read up on it more to try to get it figured out. I haven't had much time to work on it but should be able to make some progress in the next few days. Thank you for breaking that down for me and making it easy to understand.

[Anonymous]

I have more designs that are similar and when I move on to them I'll see which way is easier and makes more sense to me. 

You're right about some of the tubes being a bit overkill, especially in the rear section. The design is meant to be compliant to a certain SFI spec and it goes beyond what is required in some areas. These are areas that I felt could be improved and strengthened but I'll have to figure out how much weight they will add. Thank you for your advice, and if you have any specific suggestions I'd be happy to hear them. I'm open to criticism and always open to learn. 

[chrisplyler]

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@kb9ydn wrote:

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Most of the time I follow the one body per component rule pretty strictly.  But for things like weldments where the final product will be a solid contiguous structure, it makes more conceptual sense (to me) to treat the whole structure as a single component.  But it also depends on how you want to model the structure.  If you intend to use joints to connect all of the pieces together, then for sure you want to have each piece be its own component.  But if you're going to start with a 3D wire frame "sketch" and then apply the pipe command to the wires; having every individual piece be its own component gains you nothing.or keep track of.  The tricky part is knowing when to limit your options and when to not.

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I personally don't think that is true at all.

First, you can TREAT an Assembly with Sub-Components in it just the same as you would treat a Component with bodies in it. As far as the organizational hierarchy goes, they behave practically the same.

Second, it's not more complex at all. It's just a different line item in the Browser.

Third, what if you want to create a cut list of individual pipes? What if you DO want to Joint some pipes together (suspension components, for example)? What if want to save out certain pipes, or certain grouping (Assembly) of pipes, for use in a separate project or to explore derived variations? Etc.

If you do it my way...you definitely aren't limited further on into the work. If you do it your way...maybe you won't run into those limitations...but maybe you will. That's why I suggest just doing it all with Components from the beginning. That's why this philosophy is commonly referred to as a "Rule" in these forums.

You can often get away without it, but just as often, you're going to regret doing so.

[Anonymous]

I've still been trying to figure out my wire frame. I did about Half of the chassis and then began mirroring my sketch lines to the other side but I can't seem to mirror any of my sketches that feature lines between planes/3D lines. I can understand why because there doesn't seem to be a way to create a valid mirror line.

In the program I was using before fusion 360 I could always just use any axis of the origin to mirror lines across.

Is there a different feature I should be using to copy my 3D sketch lines onto the other side of the wire frame?

[davebYYPCU]

I think you have missed the point, yes a 3d wireframe is the end result, but

3d sketches are not required, and are hard to make.

Many smaller 2d sketches and building the pipes per panel.  When finished you would have a 3d wireframe if the bodies are turned off.

Without the file, assistance is limited to text.

[Anonymous]

I'm trying to figure out how to share the file with you as I post this. I am a fabricator/electrician by trade so certain aspects of computers are a bit foreign to me. 

I completely understand what you're suggesting with projecting planes and creating 2D sketches on each, very simple concept. I hope you're right and I'm just not getting it but it's hard for me to understand how to project planes through lines and points that don't yet exist because they will not mirror to the other side of the sketch. Thank you for your response and I appreciate your patience. 

[davebYYPCU]

It's File > Export, save locally and then attach here with the browse button below this window.

[Anonymous]

Thank you so much. Hopefully this works

[Anonymous]

On component labeled "rocker side" and "top" I can't seem to get any of the lines to the opposite side of the chassis. I did manage to get one of the diagonals by just sketching a new one based off of the points I knew it was attached on the other side