Designing plastics workflow

jboerhout · ‎05-17-2019

I have been designing with F360 for 3 years, exclusively for plastic enclosures. Learning through my many mistakes (and wasted prints), I have formulated the following workflow and would love to have more experienced eyes comment on this:

Right after creation of the new project, bring in all the objects this product needs to mechanically interact with (PCB, plugs, etc). This allows me to rely on the object's dimensions in the sketches later on.
Create the sketches.

Depending on the complexity of the design this is at least a bottom, top, side drawing but often I make drawings of just a detail part that relates to other drawings.
I use the fewest number of dimensions possible and heavily use the mirror function where I can.
All dimensions are named in the parameter list.
Additionally, I extrude bodies as I draw to test out the drawing so to say but I do not leave these hanging around and destroy all bodies so that when I am done with making sketches I have no bodies.

Extrude all bodies using the drawings are parameter list.
Apply draft (angle values from the parameter list)
Apply fillets and chamfers where needed.

The reason I work entirely from the parameter list is so that I can make changes very easily later on. Additionally, naming a dimension that occurs at several places is much easier to manage when named rather than just a value on the sketch(es). The reason I create and delete bodies during the drawing process is so that I can understand how to dimension parts (ie. where to place the hard dimensions, where the dependancies go etc.) but if I leave the bodies around they are part of the history cluttering things up/creating dependancies.

When its all done, I would like to make some sort of exploded view drawing pointing out the various dimensions (by name) but haven't been able to find how to make that process easy.

Does this make sense? Is there a better way or am I forgetting a step or two?

Anonymous · ‎05-23-2019

Only a few nitpicks, otherwise I think your workflow is fine. But if you're interested, I've seen a very interesting workflow for enclosures that you might like.

Right after design creation, you should also create a Component for all your bodies and sketches and keep all of the imported parts outside of this component - this just makes it neater when later used in another design. Most of the time I call it the same as the Design name.

"heavily use the mirror function" - Over time I've learned that this can slow down Fusion quite a bit, unless you mean the Mirror function for bodies, faces and features - which is actually prefferable.

A while back, this project caught my eye, and upon opening the .f3d files you'll see that to make the enclosure, the designer just drew the wall profile, path and then used Sweep to create all of the walls. Complicated to immediately imagine the whole enclosure and draw it like that, but extremely efficient.

https://www.thingiverse.com/thing:3338826/files

TrippyLighting · ‎05-23-2019

It would probably help to get more detailed feedback if you would share a design and maybe a screenshot that includes the timeline.

jboerhout · ‎05-23-2019

@Anonymous

Right after design creation, you should also create a Component for all your bodies and sketches and keep all of the imported parts outside of this component

Yes! agree completely. Also the attached project was interesting to look at. Doing a profile sweep is quite attractive in some designs but tough to do for more complicated things (even enclosures). This method would give better control over "ones own" draft method - I have find the F360 draft function to be unreliable/unpredictable at times.

My biggest struggle with the workflow I use is the parameter list function which seems halve baked:

* it cannot be kept open while designing

* the parameters cannot be sorted alphabetically (or some other means)

* the parameters cannot be grouped (for example by design, component or ...)

* going from design with an applied parameter back to the list to make a modification is clumsy; you need to remember the name and if you have a lot of them, somewhat similar, is a bit annoying.

It feels as if the more experienced F360 users are not using the parameter list i.e., there must be a better workflow I just dont know about. I think F360 has a lot going for it but it seems to me one must be able to create locked down designs with an efficient workflow for professional work. I dont see that happening yet. But perhaps it is just me, noob, speaking?

Anonymous · ‎05-23-2019

I very much dislike the Parameter window aswell - and since it is literally a single window parameter/container type that has to change (modal has to be changed to modeless) I do not understand why it has not been adressed yet.

Setting a keybind to the parameter window (i set it to CTRL + A because its easy to reach quickly) does help a lot when working with parameters - but even then, there are still issues once you start using complex expressions.

You can post one of your designs as a exported .f3d and I'd gladly take a look at maybe suggest improvements, but as far as I know there are no set "proper" workflows for Fusion. Just tips and opinions like:

- Split your designs into submodules as this might decrease dependencies and thus issues with the timeline when changing some parameter.

- Utilize the new "Derive" function to create a template for multiple versions of the same design - like branches.

- (my own experience) When projecting a sketch onto a body wall, use the Offset Plane if there is a change that the wall might change or even dissapear as the "redefine sketch plane" is extremely primitive and gets rid of most constraints when used.

Those were a few that came to mind right now.

TrippyLighting · ‎05-24-2019

I missed that the link to Thingyverse also included the .f3d files. Thanks! I wish more people would do this!

Looking at one of your designs I do have a few comments on your workflow. Keep in mind that this comes from the inventor of Fusion 360's R.U.L.E #1.

1. For designs that only have a hand full of components skeletal design where you might use a single sketch to create several opponents from is perfectly fine. You don't always have to start with first creating a component, it simply helps organizing the timeline.

2. While I can see the utility of putting a "complete" profile into this sketch including fillets generally I keep sketches as simple as I can and what can be modeled with solid features will be modeled as solid features. Decorative fillets such as the ones highlighted in the screenshot can be kept out of the sketch and added as solid features at the end of the design process.
Often body edges are referenced in the sketches to further build geometry and the added detail of fillets and chamfers in projected sketches is much more prone tp break projections and sketches.

3. As this is symmetric it would make sense to have the (sketch) origin located in the center. That will avoid you having to create and auxiliary mid plane for mirroring. The mirror feature in the design I am looking at is already broken 😉

4. Make sure your sketches are fully constrained and full dimensioned. The blue lines are not fully constrained and can be dragged around easily even when not actively editing the sketch. This can easily break designs and make them unusable.

5. I find adding every dimension to the parameter window is very counterproductive. That has really nothing to do with the lack of functionality of the parameter window (I do have my own wish ist). I only add parameters that I use in several different places in a design. In case of your box, most of the driving dimensions are already in your very first sketch, which is also named appropriately and easy find in this small design.

Simply right click on the sketch and select "Show dimensions" then you can see the relevant dimensions in the viewport in context and can also directly edit them there without having to actually edit the sketch.

jboerhout · ‎05-24-2019

@TrippyLighting

I missed that the link to Thingyverse also included the .f3d files. Thanks! I wish more people would do this!

Notice that the attached files were provided by @Anonymous as an example, not by me. I am simply interested in a (abstract) workflow/best practice that generally works for designing plastic components. Your comments are still appreciated though.

Over the past years I have had to waist so many designs that were incorrectly started or worked on (by me) simply because I did not understand the impact when what is being drawn etc. I have a much better understanding now and the parameter list is a central workhorse for me. So therefore, your statement:

I find adding every dimension to the parameter window is very counterproductive.

I would appreciate if you can elaborate on this. For me the parameter list allows for tweaks and nudges much easier than numbered dimensions directly in the sketches. I often design an enclosure with some dependancy on internals (i.e. the gutts) but then need to make it look estatically appealing which is all in ratios, forms and shapes even though the enclosure remains essentially what it is. Going back/forth in the sketches for that is horrible to me. So what am I doing wrong or which vehicle should I be using instead? Love to learn.

TrippyLighting · ‎05-24-2019

@jboerhout wrote:

Notice that the attached files were provided by @Anonymous as an example, not by me.

I guess I missed that as well. My bad 😉

@jboerhout wrote:

I am simply interested in a (abstract) workflow/best practice that generally works for designing plastic components. Your comments are still appreciated though.

Using a concrete example makes it much easier to explain an abstract workflow.

If you are designing geometry for injection molded plastic parts then I believe that some of the tools that would help in Fusion 360 such as the draft and rib/web tool leave ~~something~~ a lot to be desired.

@jboerhout wrote:
I find adding every dimension to the parameter window is very counterproductive.
I would appreciate if you can elaborate on this. For me the parameter list allows for tweaks and nudges much easier than numbered dimensions directly in the sketches. I often design an enclosure with some dependancy on internals (i.e. the gutts) but then need to make it look estatically appealing which is all in ratios, forms and shapes even though the enclosure remains essentially what it is. Going back/forth in the sketches for that is horrible to me. So what am I doing wrong or which vehicle should I be using instead? Love to learn.

If you remember what all of the parameters do and it works for you, then there is no good reason to work differently.

However, you mentioned a few shortcomings that are also one my wish list.

I personally find modifications in the viewport and in sketches easier, particularly when trying to find pleasing forms.

But then, I keep my sketches simple and work with solid features where I can.

If I model a solid fillet onto an edge, I can select that fillet in the viewport, right-click and select edit feature.

then the timeline automatically rolls back to that feature and the UI form that fillet opens up. When done the timeline automatically rolls back to the last position.

TrippyLighting · ‎05-24-2019

Attached is the Box design form @Anonymous earlier in this thread.

Hopefully that explains what I mean with simple sketches and features rather than more complicated sketches.

Anonymous · ‎05-24-2019

That is a really nice workflow. And I agree that (atleast until the param. window gets a overhaul) the parameters should only be used for the most used numbers that span atleast a few parts of the model - or parts that you know you might need to tweak or change in a derivation later on. For example, for 3D printing, a manufacturing tolerance is a must as a parameter IMO.

TrippyLighting · ‎05-24-2019

@Anonymous wrote:

... For example, for 3D printing, a manufacturing tolerance is a must as a parameter IMO.

While this probably does not work in every situation, for 3D printing I'd design to nominal dimensions and then offset surfaces at the end of the timeline to create the necessary clearance.

That keeps you sketches simple and clean and your design intent understandable.

Anonymous · ‎05-24-2019

@TrippyLighting wrote:
While this probably does not work in every situation, for 3D printing I'd design to nominal dimensions and then offset surfaces at the end of the timeline to create the necessary clearance.

I haven't tried that yet, and don't know how well that would hold up in my iterative design workflow. Right now I just add or subtract the tolerance variable from the sketch dimensions and other operations - works the same for sheet metal where offsets probably wouldn't. But I'll give it a shot, and see if it makes the designs clearer.

jboerhout · ‎05-24-2019

@TrippyLighting wrote:
@Anonymous wrote:
... For example, for 3D printing, a manufacturing tolerance is a must as a parameter IMO.
While this probably does not work in every situation, for 3D printing I'd design to nominal dimensions and then offset surfaces at the end of the timeline to create the necessary clearance.
That keeps you sketches simple and clean and your design intent understandable.

I do this also. But all my designs go to 3d print for verfication and then to the molder so they need draft, fillets. So I always print the final (moldable) design. It is sometimes a bit of a fight using the autodesk draft or just make it part of the drawing and then still add tolerance clearance. I am not familiar with other EDA but F360 appears rather clumsy at this - labour intense and easy to make mistakes.

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Designing plastics workflow

Designing plastics workflow

Designing plastics workflow