Custom Feature Mutual Trim

Nick_Holzem

@MBartlett21 and @Evan_Reese I'm interested to try across bodies. It seems like it would work great in cases where the intended split needed to cross multiple faces. Thanks for the further clarification - I will be sharing this with my team!

billy2

@lana and any others wanting to understand surfacing vs solids. This is a fairly common practice amongst a small community of plastics designers. Sorry, this will be a long post.

So here's the idea, create a tailpiece for a motorcycle:



I prefer working with an industrial designer to come up with the looks, in this case I did it:

There's a tremendous amount of work that goes into the 1st loft. 


The 2nd loft:

I don't think bridge curves existed back when I did this. I do tend to play with magnitudes to control my blends and I use the surface highlighting to control the smoothness.


Highlights to control blends:

This actually took some trial and error. There's a tight corner in the upper right that transitions into a body blend. It looks good on the actual part which is printed nylon but it's a fairly small part. I don't use curvature combs or any edge controls and focus on the surface highlights. I'm not saying this is correct it's just currently how I do it.


Side trim to tuck into seat:

There's always tons of prep work to build up for one trim feature (while you're at it, we need a trim feature).


And then there's the other side:

A lot a people say you can't do this, but you can.
I don't want to control both sides when designing, build one side and then mirror.
Some would object to conditions at the mirroring plane, I don't have those issues.
In this design, I have a feature that'll span across the mirror plane.


Spanning center feature:

You can control the blend between the 2 halves, but it requires planning/forethought.
I brought the tank detail down into the tail piece.


Tank detail:



All surfaces and a ton of scaffolding:



Solidify:

I rarely use shell or offset.
I find it better to build inside details manually for: ease, speed & control. 
I used enclose, as you know, it forces solidification which you have to plan for. I have an IR issued to fix this but will use mutual trim in the future.


Then there's a ton of solid features to finish things up.



This is a common workflow that I use when creating organic shapes. Surfaces differ from solids in the amount of prep work that goes into the construction of a single surface feature. With solids it's one sketch and with surfaces it's 20 scaffolding surfaces to generate the edges needed for the final surface. Scaffolding is my name for the build up of a surface. You won't find any reference to it in technical manuals.


This model is fairly robust. I put the design on my website a while back to allow someone to design their own tail piece. I controlled magnitude vectors with html input so people could change the curvatures of a custom tailpiece and my website updated to reflect the changes.

Nick_Holzem

@billy2, Great work! we follow a similar workflow at my work. Yes, we mirror about centerline! I end up using split and then follow with delete face or part to emulate a trim. 

billy2

@Nick_Holzem thanks,

It's surprising how few do surfacing. 

lana

@billy2
Thank you for the detailed explanation. This is very helpful. And I also call those reference surfaces scaffolding 

billy2

Great! it's now official. Scaffolding it'll be.

nick_papageorge073

lana said:

@billy2
Thank you for your response.
Do I understand it correctly that you would normally build one face patch at a time because multi-face loft newer gives you a sufficient control to build the shape you need? 
Please suffer me to be a devil's advocate for a bit. Making Onshape better ( including surfacing) is the ultimate goal here. I've seen enough bad geometry and horrible feature trees achieved by surface modeling. Could you please dig a little deeper into why working with surfaces is better. Let's say you have several surfaces defining a shape, you used Mutual Trim and got closed surface. What do you do next?
Other surfacing users - please join the conversation. I'm looking to understand the organic modeling workflow better.

I designed parts for injection molding for 15 years using ProE/Creo at a baby products company. (car seats, strollers, high chairs, swings, etc). Everything was done in surfaces. Even when the shapes weren't "organic". Its because its the nature of injection molding. You want a constant wall thickness. You also need to have explicit control of the parting line. For example if you model a part as a solid with draft, then shell it, the parting line will be normal to the draft, rather than normal to the draw direction. Conversely, if you draw each surface, including the parting line, you have much more control.

One other reason it was all done in surfaces is you could only publish geometry from a skeleton model in creo if it was drawn as surfaces. With OS having multi-body modelling, maybe that negates some of that.

When I would do a part, I'd typically model the show surface of the part as a quilt (in Creo terminology). (multiple surfaces merged together). Then offset that surface the nominal wall. Then I'd have the outer and inner main surfaces of the part. Those won't be merged together with the side walls until much later in the tree. Now, I can work on individual features, such as ribs, bosses, bypassing steel shutoffs, etc. Some of those features will get merged with the inner wall, and some with the outer wall. Doing it this way gave a ton of control.

The caveat to this is since switching to OS a year ago at another company, my parts are way simpler than injection molded parts. I have thermoformed parts and sheetmetal parts. OS is working great for them. I'm not sure how I'd attempt to model a complicated product for mass production consumer use made with multiple injection molded parts fitting together.

I kind of wish you had a real, fully designed product, in your tutorials, that was completely injection molded. You have the clothes iron, but its only the basic shell. I mean the whole thing fully done.

billy2

@nick_papageorge073

I agree, there needs to be more education about designing injection molded parts. It should probably start with how an injection molding machine works.

You can create multiple injected parts inside OS. I'd probably do it inside a partstudio because all parts could share common references easily. It'd be a long feature list and you'd would have to manage the tree otherwise things would become chaotic. If you have multiple injection molded parts I'd absolutely do them in a part studio so I could easily share datums between parts. I'd also build an assembly so I could check the movement between parts. Top, bottom & battery door snap latch; I've done this a dozens of times and use a another assembly to stuff in the electronics.  I'd avoid incontext (or designing in the assembly) because moving parts mess up common references. An easy way to think about a part studio is having incontext without any moving parts. With multiple injection molded parts I think OS could do a very good job. Give it a try next time and let us know how it goes.

If you have a production injection molded part with 100's of functioning features, the model would be complex. One of the problems I see is that people are just stacking features on top of one another without reordering creating logical groupings of features so they end up with a long list of un-maintainable features. I have no idea how these guys handle change and I believe they start over.

I'm printing most of my parts today because I don't have the volumes to justify making an injection part. I've printed qty 2 of the part tailpiece and that's probably it. I do design a lot of stuff and make qty 1 of a most my stuff. With nylon, flexural modulus and some FEA you can design snaps that work and a lot of cool stuff. I don't worry about drafts, undercuts & slide shutoffs any more and I don't miss it. Designing printed parts is a lot easier than injection molded parts.

Can you post a picture of one of your complex parts? 

nick_papageorge073

billy2 said:

...snip...

Can you post a picture of one of your complex parts? 

I wasn't on the carseat team, but have seen their cad models and talked with their engineers. A carseat is typically 3000-5000 features, with about 1000 of them being rounds. It can't be broken up because its one injection molded part. This is in ProE/Creo.

Here is a product I worked on in 2006 I believe. I did the whole housing in ProE, the other team members did the other areas of the product. These pictures are screenshots from my resume/portfolio, so they are semi-public, and the product has long been discontinued... I vaguely recall the skeleton model was maybe 1000 features. And then when transferred to the subsequent components, they each had a several hundred features additional. I do believe OS would have allowed the same design in much fewer features.

lana

@nick_papageorge073
Thank you for sharing your process and the examples.

billy2

@nick_papageorge073
Thanks for showing these, I wish I could see your feature tree and would love to see how you setup your datums and control structures. Can you share your pro/e model?

I'm supposing skeleton surface model translates to a knitted surface body? I'm not certain the word "knit" is used any longer. In onshape you just boolean a bunch of patches together to form something. I'm not sure what it's called now.

Boolean patches create what?


My pro/e understanding, the word "skeleton" was a top level assembly structure to help bring order to large assemblies. I'm sorry but my pro/e knowledge has rusted about 25 years. I'm definitely interested in how pro/e controls plastic part designs.

I've seen guys go from surfaces --> solids --> surfaces -->solids which I consider bad form and the result of a snowball of features. There's a lot of that going on out there. Does pro/e stop that workflow? Once you convert your skeleton to a solid, can you go back to surfaces?

In onshape I have a habit of creating control features out of surfaces, I change their color to transparent yellow and leave them in the surfaces folder. At the end of a project, the surface folder contains only control surfaces used in the project. A temporary surface that's not a control object is deleted after use keeping the surface folder containing only control structures. I manage the surfaces in my surface folder. This is something I do. If you want to know how something's controlled, you just show the surfaces folder then you can easily find the control and drill down to the specifics on how a feature was created.

billyCAD 101 control surfaces:


We don't have dedicated control structures and I make do with what I have, I'm not complaining, its working fine. I gave up on datums & axis many moons ago due to the fact they don't translate. My solidworks models came into onshape with all control structures (because they're surfaces) which really helped when migrating data into onshape. I've been using surfaces for datums for a long time. I had a complex non-planar parting surface which was translated into onshape making it managable to continue. There are things that are almost impossible to recreate from a translated data set. If you use surfaces, which do translate, in the new system, you can continue the design in your new CAD system.

Have you ever exported your pro/e to another CAD system to see what you get?

If you have a current pro/e plastic assembly that's not under NDA,  if you can step it over to me, I'd love to poke around and see what I receive. Just PM me and I'll give you my email address.

MBartlett21

@lana

Could you have it remember the previous boxes for merging and making solid please?

lana

@MBartlett21
Done https://cad.onshape.com/documents/342ea79aa4fd6b12b9863cc4/v/3f23972ad197d54c32e40df7/e/56b1ebc53519161a34c02cea
Making solid was remembered before this. 

MBartlett21

@lana Thankyou

lana

A new version of Mutual Trim released to take advantage of an edge tracking improvement in rel-1.147 deployed yesterday.

EvanReese

Thanks for ongoing improvement and maintenance of this feature, Lana!