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Dominoes
Sep 20, 2007



I appreciate the wisdom! Going to keep the assembly, minus the enclosure top, which is now part of the enclosure bottom. Should I just delete the enclosure-top part file? Seems like there's no good way to sync things otherwise.

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NewFatMike
Jun 11, 2015



Check out this help article, it'll give you the full picture:

http://help.solidworks.com/2020/English/SolidWorks/sldworks/c_Split_and_Save_Bodies.htm?verRedirect=1

The important part, though, is this:

quote:

If you change the geometry of the original part, the new parts also change. If you change the split feature geometry, no new derived parts are created. The software updates the existing derived parts, preserving parent-child relations.

E: happy to help! I'm a massive proponent of the Makers program, I came up from a non-engineer background, and I wicked love being a nerd about CAD.

Dominoes
Sep 20, 2007



I appreciate it. It looks like there's single-direction change propagation; ie you still need the old part file, and edits there affect the new thing. But joint parts like latches must be done on the multi-body parent, and don't propagate to the child; just like you said.

NewFatMike
Jun 11, 2015



If you do something like edit the dimensions of your snap hook and groove feature, then it ought to propagate to the child.

All new features would have to be done above the feature that splits and saves, so you would use the rollback bar to do it.

I.e. you split and save a part, use the rollback bar to get above that split and save, pull the rollback bar back down, and the child parts should update.

Yooper
Apr 30, 2012



Grimey Drawer

Argh, gently caress me.



Joints gone wild. I guess I won't do a bellows like that.

biracial bear for uncut
Jun 9, 2009

ask me about being the most obnoxious person of all time

Probably need fewer and longer segments for that to work the way you want it to.

Sagebrush
Feb 26, 2012


"Why does that Subaru break down every time you look at it, Travis", Punchy said. I nearly fell out of the jump seat in my Brat, aghast. "That thing a princess?" I coughed and gulped. "Hahahaha, nice one, Punchy", I said

Honestly that's kind of what I would expect bellows like that to do if they aren't constrained to move along a track.

Maybe try putting a sort of sliding pin in the center of each slat, and constraining that to run in a horizontal track?

Ambrose Burnside
Aug 29, 2007

pensive


Sagebrush posted:

Honestly that's kind of what I would expect bellows like that to do if they aren't constrained to move along a track.

Maybe try putting a sort of sliding pin in the center of each slat, and constraining that to run in a horizontal track?

Ding ding ding. Pins and slots are probably easiest. Alternately you can maybe use a self-constraining linkage structure like pantograph bars, depending on the overall design. Probably a bigger pain in the rear end, but linkages are the poo poo and people oughta tackle designing them at some point, pay respect to the old masters and all that. Also they’re fun. and it’s really hard to gently caress up a panto/scissors linkage compared to a proper straight-line linkage mechanism.

Ambrose Burnside
Aug 29, 2007

pensive


EE/circuit CAD question: what program is a good fit for designing PCB traces if my design parameters are very different from conventional circuit design, and the resultant traces look very different from standard trace conventions?

I’ve experimented a little bit with what a i call “plotter/drag-knife flexible circuit boards”- it’s a potential cheap and easy way to produce CAD-derived circuits using just a Cricut-type digital plotter, the ‘trace’ is cut from conductive copper tape and the ‘board’ is thin but springy Mylar sheet, with transparent adhesive film added over the copper if the traces need to be insulated /physically-protected. thru-holes in both parts are used for alignment/registration and the copper trace is lifted off the tape backing and onto the backer sheet all at once using transfer film.
The end result is flexible and durable and can even be soldered to, but I rapidly found that standard trace geometries/proportions are too fragile for the process- the transfer step easily tears the tape, so very proportionally-chunky, oversized traces with no sharp corners (i.e. tons of filleting needed b/c tears propagate from hard corners) are called for.
I tried laying my own out in a vector graphics program but gave up pretty quickly because it was an incredibly slow way of working. I have zero proper electrical CAD experience. What’s a good beginner-friendly software option that’ll specifically let me design my own custom trace ‘template’ /scheme based on dimensions/ relations, so I can design a circuit without having to do hours of vector graphics gruntwork?

His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


I'm looking at library features in solidworks. I was thinking of having a bunch of mortise and tenon templates ready (for use with the pantorouter). I started wondering if you need to model the mortise and tenon, maybe it'd be better to store just one feature as a 2D template, then you can import it onto a feature and extrude it as a mortise or tenon depending on what you want. Since you might want to vary the depth of the mortise and tenon from time time.

NewFatMike
Jun 11, 2015



You can override dimensions in any library feature you make, so there's not really any need to get too clever with it.

The way I would get clever with it, though is, I would use the same sketch in creating the mortise and tenon, just using an offset. That would let you use the same dimension in sizing both.

I would also locate them using center rectangles using a coincident relation on a point from another sketch, kind of like how the hole wizard does it.

That means you could do a few sketches (or one 3D sketch if you're feeling real sassy) which just have points on the relevant faces.

His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


NewFatMike posted:

You can override dimensions in any library feature you make, so there's not really any need to get too clever with it.

The way I would get clever with it, though is, I would use the same sketch in creating the mortise and tenon, just using an offset. That would let you use the same dimension in sizing both.

I would also locate them using center rectangles using a coincident relation on a point from another sketch, kind of like how the hole wizard does it.

That means you could do a few sketches (or one 3D sketch if you're feeling real sassy) which just have points on the relevant faces.

Isn't that sort of the same as what I was saying, except using the extrude function. Or is there a practical difference?

Anyway I figured I could use SW to also create template geometry for me. Any mortise and tenon I wanna cut on the pantorouter has to have a template made first. The template has to be 2x the scaling and factoring in router bit size and follower size. So I made the sketch for a double tenon and then for the template. Nice thing is everything is now related to each other so if I change the size of the follower, or the router bit, or size of the tenons, the template adjusts properly. I can just get the dimensions and write them down, or print a 2d template to cut out from.



Template scaled up:

His Divine Shadow fucked around with this message at 15:46 on Apr 11, 2021

NewFatMike
Jun 11, 2015



Ah, I may have misunderstood. My (pre caffeinated) read was that you were just going to insert a sketch as a library feature and extrude a boss or cut from there.

His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


NewFatMike posted:

Ah, I may have misunderstood. My (pre caffeinated) read was that you were just going to insert a sketch as a library feature and extrude a boss or cut from there.

I think you understood correctly then, I was the one who misunderstood, despite four cups of coffee today so far. I think I understand you now though.

His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


By the way, when I radiused the corners I used fillets, but if I used the formula width of tenon / 2 then I could not use two fillets to create one radius. I had to remove .05mm from each fillets radius or Solidworks complained. I was used to doing it the way I mentioned first from Fusion 360. Is there a better way to radius the edges so I get a true radius that is half the width? This feels like a bit of hack.

Sagebrush
Feb 26, 2012


"Why does that Subaru break down every time you look at it, Travis", Punchy said. I nearly fell out of the jump seat in my Brat, aghast. "That thing a princess?" I coughed and gulped. "Hahahaha, nice one, Punchy", I said

You mean doing something like this?



It should work fine as long as your math is correct. Maybe you had a rounding issue or something.

Incidentally I enjoy that SolidWorks specifies the fillet radius to 10 picometers. Half the radius of a hydrogen atom.

His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


Exactly like that except I did it on the 2D sketch. I used formulas so that it would take the width of the part and divide it in two, should have worked...

Sagebrush
Feb 26, 2012


"Why does that Subaru break down every time you look at it, Travis", Punchy said. I nearly fell out of the jump seat in my Brat, aghast. "That thing a princess?" I coughed and gulped. "Hahahaha, nice one, Punchy", I said

Oh, you can't do it in the 2D sketch. When you sketch-fillet two corners to exactly half the width of the edge, the resulting line entity in between the new fillets would have zero length, so SolidWorks disallows it.

You can either use the arc tool to create your round cap in the sketch, or leave it square and do a fillet feature in 3D.

biracial bear for uncut
Jun 9, 2009

ask me about being the most obnoxious person of all time

His Divine Shadow posted:

By the way, when I radiused the corners I used fillets, but if I used the formula width of tenon / 2 then I could not use two fillets to create one radius. I had to remove .05mm from each fillets radius or Solidworks complained. I was used to doing it the way I mentioned first from Fusion 360. Is there a better way to radius the edges so I get a true radius that is half the width? This feels like a bit of hack.

The best way to do that is using the Fillet Feature. Best practice is to keep your sketches as simple as possible and have your complex patterns/etc. at the feature level, generally speaking.*

And in your specific case, you'll want to use the Full Round Fillet feature option and pick the left, top and right surfaces as your reference surfaces and let the feature calculate the fillet radius.

EDIT:

Like this



The "Side Face Set 2" pointer is pointing at the surface on the back of the part, but it's hard to get a good view of that in a 2d screencap. If you duplicate what I did here you'll be able to rotate your view and see what it's actually pointing at.



EDIT #2: *I say this because one of the "quirks" of Solidworks (heh) is that the more calculation you load into a sketch, the more time it takes Solidworks to process during rebuilds vs. simplifying things out into distinct features. This can make for a lengthy feature tree depending on how complex a part you're making, but then again, that's what design iteration and planning is for.

biracial bear for uncut fucked around with this message at 11:12 on Apr 12, 2021

His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


I don't know, just this sketch here won't ever get used in a proper 3D model I think. I am just after it for the 2D dimensions. I am just using solidworks here as a cheat sheet, so all the math is done for me, I can probably just write the results down on a paper and then make the template on the tablesaw from plywood. Still even so the purpose is just to generate a template and not be used as a feature in some other design. So it'll always be very small and contained.

But I get your drift about keeping the sketches simple. Not really the way I feel comfortable thinking, always wanted my sketches to be as detailed as possible and do as little after the fact modification, but maybe that was always the wrong path to take even in other programs like fusion which I am most used to.

biracial bear for uncut
Jun 9, 2009

ask me about being the most obnoxious person of all time

His Divine Shadow posted:

I don't know, just this sketch here won't ever get used in a proper 3D model I think. I am just after it for the 2D dimensions. I am just using solidworks here as a cheat sheet, so all the math is done for me, I can probably just write the results down on a paper and then make the template on the tablesaw from plywood. Still even so the purpose is just to generate a template and not be used as a feature in some other design. So it'll always be very small and contained.

But I get your drift about keeping the sketches simple. Not really the way I feel comfortable thinking, always wanted my sketches to be as detailed as possible and do as little after the fact modification, but maybe that was always the wrong path to take even in other programs like fusion which I am most used to.

You can use the Drawing side of Solidworks to populate the printout to let you know what the radius calculates out to.

Sketches in Solidworks are not Drawings (though you can make links between data in the one to populate tables/etc. in the other, Solidworks treats them as separate things and they serve different purposes). Separate the two in your mind and you'll save yourself a lot of grief going from old school drafting habits to 3d modelling habits.

oXDemosthenesXo
May 9, 2005


Grimey Drawer

You can also play with the printer settings to print the drawing at 1:1 scale. I do this once in awhile to create templates to trace.

It works best if you delete the drawing format so it's just the part/assembly left to print.

Sagebrush
Feb 26, 2012


"Why does that Subaru break down every time you look at it, Travis", Punchy said. I nearly fell out of the jump seat in my Brat, aghast. "That thing a princess?" I coughed and gulped. "Hahahaha, nice one, Punchy", I said

His Divine Shadow posted:

I don't know, just this sketch here won't ever get used in a proper 3D model I think. I am just after it for the 2D dimensions. I am just using solidworks here as a cheat sheet, so all the math is done for me, I can probably just write the results down on a paper and then make the template on the tablesaw from plywood. Still even so the purpose is just to generate a template and not be used as a feature in some other design. So it'll always be very small and contained.

But I get your drift about keeping the sketches simple. Not really the way I feel comfortable thinking, always wanted my sketches to be as detailed as possible and do as little after the fact modification, but maybe that was always the wrong path to take even in other programs like fusion which I am most used to.

The proper SolidWorks methodology here is to build the part entirely in 3D, using all the constraints and relations and automatic equations that you need, then create a drawing document from that part that updates whenever the part is changed. You can then save the drawing as a PDF or whatever to use as a 2D template.

Remember that the core file type in SolidWorks is the Part, and everything else builds on that. Sketches are just internal construction elements. 2D drawings are derived from 3D models.

Sagebrush fucked around with this message at 22:48 on Apr 12, 2021

Dominoes
Sep 20, 2007



I fired up Fusion again to see how it compares to SolidWorks now that I'm more comfortable with CAD. It won't run until I download a new version. The options are "Download new version", and "quit". Harmless on its own, but contributes, along with the cloud-saving, that this is a SAAS.

Dominoes fucked around with this message at 01:57 on Apr 14, 2021

His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


Dominoes posted:

I fired up Fusion again to see how it compares to SolidWorks now that I'm more comfortable with CAD. It won't run until I download a new version. The options are "Download new version", and "quit". Harmless on its own, but contributes, along with the cloud-saving, that this is a SAAS.

I dunno what SAAS means but I like to imagine it's something like Sucks rear end And poo poo.

Case in point I got this model I shared once on the autodesk forums of a tri-axial hinge and people keep PM'ing me years after the fact if they can download it so I had a link so I could share and they could download. But just now this no longer works, sharing files so they can be downloaded is a pro-only feature now.

gently caress autodesk, gently caress Fusion. I'd rather pay 40$ a year for this student edition of solidworks than use fusion for free.

Rexxed
May 1, 2010

Dis is amazing!
I gotta try dis!



His Divine Shadow posted:

I dunno what SAAS means but I like to imagine it's something like Sucks rear end And poo poo.

Case in point I got this model I shared once on the autodesk forums of a tri-axial hinge and people keep PM'ing me years after the fact if they can download it so I had a link so I could share and they could download. But just now this no longer works, sharing files so they can be downloaded is a pro-only feature now.

gently caress autodesk, gently caress Fusion. I'd rather pay 40$ a year for this student edition of solidworks than use fusion for free.

It's Software as a Service (subscriptions), so yeah, you're right.

Dominoes
Sep 20, 2007



It's a California / Hacker News term for a webapp, often in the form of a ponzi scheme - startups make these things for other startups, ad infinitum. If you're really successful, a FAANG buys your SAAS, and do it again, but this time you're rich.

Dominoes fucked around with this message at 22:52 on Apr 14, 2021

Dominoes
Sep 20, 2007



Got the SW O-ring revolved cut working like you said. Much nicer! The groove tool doesn't move with your geometry, as least by default (non-parametric?), and it's easier to reason about the dimensions if you're not in industry this way. Ie make the revolved circle a fixed radius, and distance from the center, instead of picking an ISO or ANSI number.

e: SolidWorks is really polished. It's clear they spent a lot of time going back-and-forth with users (internal or external) over the years to make the UI intuitive. I hope FreeCad get there eventually, but so many OSS projects get bogged down in clumsy PR processes etc. For example (Maybe I'm projecting too much from my own software projects) - User wants to be able to easily set a dimension based on something in a different sketch. They call SW dev and explain. Dev changes some code, pushes patch, and it's done. OSS: person makes issue or PR. Devs take 3 weeks to get to it. Question why you'd want this, nitpick code style and mention alternative approaches, then vanish again.

Dominoes fucked around with this message at 18:39 on Apr 19, 2021

armorer
Aug 6, 2012

I like metal.

Dominoes posted:

It's a California / Hacker News term for a webapp, often in the form of a ponzi scheme - startups make these things for other startups, ad infinitum. If you're really successful, a FAANG buys your SAAS, and do it again, but this time you're rich.

This is an emotionally charged hot take. Software as a service is not inherently any of that, although it certainly can be.

When "cloud computing" started to take off, the industry needed a way of differentiating cloud stuff, so they came up with the terms "Infrastructure as a Service (IaaS)", "Platform as a Service (PaaS)", and "Software as a Service (SaaS)". These terms have been globally accepted and used for like a decade now. They're not hacker news buzzwords. IaaS essentially covers service offerings from Amazon, Google, Microsoft and the like that let you say "Hey I need 30 servers" and then in 5 minutes or so you have 30 servers in the cloud that you can mess around with. PaaS takes you a little bit further from the metal, and lets you say "Hey I need a 10 node Postgres database cluster" or "Hey I need this particular webserver stack so I can deploy a packaged Java application" and then in 5 minutes you have that thing.

SaaS is exactly what it is named - software as a service. You are delivered the use of some software using a service model rather than a (historically more conventional) ownership model. Facebook, gmail, instagram, snapchat, gently caress even the SA forums, are ALL Software as a Service. You don't own the software, you may have paid but may not have paid, and you are able to use the software according to some terms of use.

What Dominoes is getting (to some extent rightly) mad about here are software products that used to follow a "shrink wrapped software" distribution model whereby you would pay once and then own the software. There was an inbetween time, after the internet but before the widespread adoption of the SaaS model by big software companies where you would buy the software, but then in order to get updates you would need to pay for a support subscription. That model has essentially been phased out in favor of just having you pay a subscription and never owning the software at all. That model tends to gently caress over the consumer, because while you do gain the advantage of continuous updates and generally some cloud enabled features like file storage or other perks, you end up paying a lot more over time than if you would originally have just bought the software once and not paid for support.

That is not an inherent evil of Software as a Service though. The mobile computing experience as you know it today is powered almost entirely by the SaaS model, and on the whole it has done way more good (by which I mean provided way more capability for free) than harm (by which I mean cost more money) to end consumers.

Dominoes
Sep 20, 2007



Great explanation.

For some context, I've built and maintain what could be called a SAAS; a scheduling/training/manning web app for fighters, used by a handful of USAF sqs. Bro-level SAAS?

There's a continuum between web page and SAAS, where someone's geocities page is the former, a Silicon Valey (SV) startup that sells to other SV startups is in the latter, and other websites can be categorized in a way that's useful to your purpose. While a desktop software, Fusion 360 behaves in some ways that are associated with SAAS sites.

Dominoes fucked around with this message at 18:17 on Apr 19, 2021

Sagebrush
Feb 26, 2012


"Why does that Subaru break down every time you look at it, Travis", Punchy said. I nearly fell out of the jump seat in my Brat, aghast. "That thing a princess?" I coughed and gulped. "Hahahaha, nice one, Punchy", I said

Dominoes posted:

e: SolidWorks is really polished. It's clear they spent a lot of time going back-and-forth with users (internal or external) over the years to make the UI intuitive. I hope FreeCad get there eventually

lmao. I think this speaks more to the utter shitpile that is OSS user interface design than anything actually good about SolidWorks, lol

like yeah I prefer SolidWorks over any other solid parametric modeler, but I've been using it for nearly twenty years and I'm fully aware of its conventions and quirks. There are so many dumb hacks and useless error messages in the program and you just learn eventually how to avoid making them happen.

"feature failed due to geometric condition" hell yeah i love useful information

"the feature could not be created because it would result in zero-thickness geometry." no, actually, it would result in two coincident edges, which is totally fine for a solid model, and i know precisely what i'm doing. thanks for helpfully stopping me though

"this feature cannot be patterned with the geometry pattern option. try deselecting the geometry pattern option" oh ok so you know exactly what the problem is but you still haven't fixed it after literal decades and just pop up an error saying don't do that. great

or the way that the feature tree moves to the inside edge of the viewport when you have a property page open, because both of those things share the same screen space but oooops sometimes you have to use both at once. redesign the UI? gently caress no, just uhhhhh stick that over here sometimes i guess. bing bang boom

like yep i still will use it first and i'm quick with it but whooooooooooo


armorer posted:

That model tends to gently caress over the consumer, because while you do gain the advantage of continuous updates and

just incidentally I loving hate the automatic updates. that's fine for instagram or whatever but when it's software I use every day, DON'T gently caress WITH IT. I started up KeyShot today and oh it updated last night and broke a bunch of custom file associations and material folders I had built. thanks. love it. shithead

adobe is even worse about it. new update every week and who knows what it's gonna do this time!

Sagebrush fucked around with this message at 18:41 on Apr 19, 2021

armorer
Aug 6, 2012

I like metal.

Yeah so just to be clear, the "as a Service" part is the main differentiator here. You can have Software as a Service that is still delivered as desktop software, although most of it takes the form of either a webapp or (in the case of mobile) an app. Fusion 360 is SaaS that is delivered as desktop software, but is closely tied to the backend in that it calls home all the time for updates, license checks, etc, and also has some cloud enabled features where you can invoke some menu function in the desktop software that actually then gets computed in the cloud rather than on your machine. That last sort of feature tends to have a correspondingly poor user experience because of weird latency issues (and the fact the user often doesn't know it's happening in the cloud, and thus expects the same sort of instant response they would get otherwise.) Well managed SaaS will enable a company to do things like push fixes for security vulnerabilities, add features over time, improve UI/UX based on user feedback, etc. In practice, a lot of companies do things like push new features that break customizations (like Sagebrush is mentioning above). Netflix constantly analyzes user data and tweaks the UI to minimize the number of clicks needed to get to the stuff they want you to watch (and also hopefully the stuff you want to watch).

Basically I'm just trying to make it clear that the 'aaS' part essentially refers to the delivery model, and isn't really inherently good or bad. I personally think it enables a lot of really cool things that we use all the time today, but I also recognize that it's poorly implemented, frustrating, and expensive in a lot of other cases.

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His Divine Shadow
Aug 7, 2000

I'm not a fascist. I'm a priest. Fascists dress up in black and tell people what to do.


One thing I like about Fusion 360 is when I try and rotate the view it, it just works, like intuitively. When I rotate something in solidworks or solid edge for that matter, the model just seems to also rotate in multiple random directions plus the one I intended and I can't make heads or tails of it and it's so incredibly frustrating.

Fusions way of rotating the view just works so bloody well.

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