This is to get a conversation going about your favorite method. Why do you use it? What are the limitations? What are the important features? Do you evangelize?
-Top Down using Save Bodies
-Top Down Assembly-based
-SSP
-Bottom Up
-A hybrid approach
-Or something totally different?
Ditto. I have deserted that road too.
Someone should make a meme for that.
"Oh, you use Save Bodies? I also like to live dangerously."
I design small machines - power tools. My technique from your list would have to be Bottom Up. For the moving parts and ranges of motion I will often make sketches in the assembly, but ultimately the design and function of the parts themselves is what I'm after. Occasionally I'll make an assembly cut that I propagate to the parts, but soon after that I'll make those features independent in their respective parts.
Some folks are die-hard advocates of mating on primary planes. I'm not. My parts are mated on the surfaces that will actually be used in the assembly. I take advantage of flexible subassemblies and their ability to have Limit Angle or Limit Distance mates (think of a pneumatic cylinder). Gear, and Rack and Pinion mates are of great value to me as well.
Ayyy Yayyy Yaaayyyyy!
Don't forget:
- Master Model
- Layouts
- Resilient Modeling
- Skeleton Modeling
- Horizontal Modeling / Wide Tree
- incontext without relations
- Synchronous Assemblies
Master Model Part 5: Best Practice and Horizontal Modeling
Resilient Modeling Matures – Interview with Dick Gebhard
Synchronous Assemblies Brief Demo
Huge topic. Software developers don't understand it or at least have not provided a solution that isn't disastrous.
I'm not quite ready to 'evangelise' my technique as there's still a few wrinkles but I use something I call 'Blue Box' modelling.
It's an SSP based assembly technique - but you won't see a single sketch.. its more a Skeleton Surface Part
The SSP serves a few functions.. it provides the default planes and surfaces that are used to mate the parts to whilst also providing the key dimensions and the equations that size the general layout.
I always try and lever configurations, so that the same skeleton can be used to control multiple configs as required.
In the assembly the skeleton is always the first component and is set to envelope
The SSP is also inserted into the components - here they are all different configurations of the same part, but this is not required.
No model geometry is inserted.. only the model dimensions.. which can be used directly to calculate the size of each piece within the assembly.
I always use a lot of configs and configured equations
For example here is two of the configured subs together.. all from just 2 parts, the skeleton and the stuff
I have a custom Add In that handles surfaces in the part that are used instead of planes - think of it as a surface bounding box.
There's a bit more to it.. one of these days I might make 'Blue Box' tutorial that's fit for sharing.
Key points
Everything modelled around default planes.
Surfaces used in lieu of conventional reference geometry
SSP used as envelope
SSP model items inserted into parts
Heavy use of configurations
Some custom macro features
Apart from configured configurations the assemblies are dumb.
The general layout is all done in the SSP
The fine grain details are done in the component
Some benefits
Hardly any files
No external reference of geometry to break (It's all in one part)
Surfaces always appear in the correct location and surface faces cannot be cut/lost
Use of colour schemes to colour surfaces
Any changes or new features are available for all configs instantly
A formulaic approach to modelling that is consistent between models but flexible in use.
Downsides
Requires care - all eggs in same basket
Solidworks is sometimes unreliable with configs - NEVER use a derived config
Primarily tailored to 'Boxy' models - lucky for me that's what woodwork is!
Ooops that ended up longer than I thought.
Looking forward to following this post
[edit] forgot the most important part NO mates or references to ANY actual model geometry
Its all done with the blue box - the model geom is free to be anything
Master Sketch. A Master Sketch part file is inserted to every parts.
Assembly could have the Master to mate parts.
Which ever way I need to get it done. Top Down, Bottom Up, Inside Out.
Currently I mostly make fixtures, welding, machining.
So it'll start with customer models for locating points.
I appreciate all your replies and insights. And now to insert my opinions/beliefs/worldviews/dogma...………
To give a bit of background- we use mostly structural weldments and sheet metal to create welded assemblies that are used later in a Final Product Assembly.
We have been on quite a journey here. The previous "engineer" (long story, ugh) basically used Bottom Up. Next we started using Top Down with Save Bodies. THAT got ugly really quick! I'm still fixing problems a year later. The biggest issue was dealing with part configurations that lost their references later.
Now we use a hybrid approach. Anything that is welded together is modeled in a single part file. We use Cutlist Properties for part no, desc., name, etc. Then we create an assembly with all the different welded parts (i.e. base frame + guards + vendor components). We generally don't use external references and Inplace mates in assemblies.
Pros:
A welded part is all done in a part file context for maximum modeling efficiency.
Very stable with few crashes and short rebuilds.
Easy to understand from an outside perspective.
Cons:
Not as parametric as Assembly Based or Save Bodies (references between separate welded components).
Cutlist properties are tricky to get onto a title block in a drawing.
Using shared components between models is more difficult (either copy the sketch or insert the stand-alone part later in a lower level assembly).
Pinging:
A few things I have learned to increase stability when changes occur:
-use Fillet feature instead of Sketch Fillet
-reference Linear Patterns from primary planes as much as possible
-keep origins centered on parts
-mirror, mirror, mirror, and mirror!
Dennis Dohogne wrote:
I design small machines - power tools. My technique from your list would have to be Bottom Up.
Ditto for me except my machines go from fairly small, desktop size, to "you gonna move a house with this?"
Machines are complex and will have S/A's, with S/A's and multiples of them. Every project is different and most of the time significant different. In the last three months we shipped a test machine that sways a 5K product back and forth for marine testing, a dual spindle machine for machining both ends of rollers that range from 3" to 7" in dia up to 120" long and am currently getting ready to release a machine that mills human bone into chips.
I've looked at other approaches but have never been able to wrap my head around how they could be effectively implemented for what I do.
I tend to start with the main assembly and decide where the origin should be, spindle center, table center etc. From there my S/A's are designed around the origin of the S/A being where it will be positioned in the top level. There are some draw backs to this in that the position of the S/A's do not move if the S/A they are mated to changes position. However I've found that having this break at each S/A level makes it easier to hunt down position issues and interactions of main S/A's
When I worked in Inventor I did a WHOLE lot more part to part relationships. My assemblies would generally update entirely by changing driving dimensions. My experience in SW doing this has been less than stable so I don't do that anymore.
One thing I hate hate HATE about SW is that you can't have solid or surface geometry in an assembly. This requires use of phantom parts (e.g. "envelopes", "skeletons") to maintain master surface geometry. This presents a host of file management issues (and sometimes personnel management issues).
Michael Miller wrote:
-mirror, mirror, mirror, and mirror!
Was this meant in sarcasm? In my experience Mirror in SW is about the most unusable and unstable thing I've ever seen in a piece of software that has been released for regular usage. In my experience it actually get's it completely wrong in a significant number of cases. I've seen parts that mirrored part correctly and part not.
One practice I champion but have not been able to widely evangelize is separating the design context from the product definition.
One design layout can define many dimensions of products and variations, along with positions, analyses, layout parts, and the like. trying to maintain a single product's BOM in this context is a never-ending chore.
Just make a separate assembly that is the product as-built/sold/serviced. Seems redundant, but I find it saves far more time than it seems to waste.
First I'll get this off the chest.... I use the Skeleton Sketch Method, which in reality is kind of like an open source or free wind type of modeling, basically using one component or a series of similar components that control the entire model. The SSP is a confusing acronym, because most people think you can only use Sketch Geometry, not true, you can use Sketch Geometry, Surfaces, Planes and Solids to control the entire model so that you can achieve parametric movement and changes. The basic theory behind the SSP is building a process that is repeatable giving you similar results every time, when that happens your modeling time decreases and your confidence increases...
Like everything else, it is only as good as what you set it up to do, time spent up front is time saved later. Following the SSP instructions basically saves a lot of time in overall design time, much faster and a lot more robust, it is easier to do diagnostics on parts or assemblies that throw errors.
Having said that....
There is "No" perfect system and each company has their own way of operating and refuse to change their operation to match the software that they choose to use, making it very difficult for the Engineers and Designers. Design your company system around your software for optimal results..
Send me one of your models and I'll tell you how well it was modeled, delete a part in the feature tree and see what happens..
Use SW and optimize your workflow..
I would love to show you the correct way to use the SSP, show me the money and let me know when you want me there, I'll travel
Matt Juric wrote:
Michael Miller wrote:
-mirror, mirror, mirror, and mirror!
Was this meant in sarcasm? In my experience Mirror in SW is about the most unusable and unstable thing I've ever seen in a piece of software that has been released for regular usage.
Is this because you fall into the trap of trying to mirror features instead of bodies? Sometimes features are useful, but I generally mirror bodies, and you can't ask for anything more stable than that. Especially if you aren't trying to mirror fillets. Geometry pattern is ok if you understand how to use it, but bodies is best. Mirroring bodies is much better than mirroring sketches or doubling the number of features or size of sketches.
Roland Schwarz wrote:
Just make a separate assembly that is the product as-built/sold/serviced. Seems redundant, but I find it saves far more time than it seems to waste.
The "Best Way" - done it many times, makes it much easier downstream and cuts out a lot of SW issues when dealing with Configurations or Design Tables at that level
Awesome stuff, I wonder why I'm turning Green
Lately, I have been using a Master model mixed with a little bit of SSP. Although when dealing with other designers, this can become a headache.
Then I split the master model into parts (1 body per part) and assemble it with purchased components.
Then create drawings.
Although it looks like I am going to be pulled away from designing for a bit because it looks like they are going to make me the plant wide PDM admin (once we get it up and running).
Although who am I kidding, I will probably be expected to do my current job AND That one at the same time. LOL
John, with SSP, does each part file use a copy of the master part or is each part defined and located by the master in an assembly?
John Stoltzfus wrote:
I wonder why I'm turning Green
All them configurations making you feel sick?
All of the above who has contributed so far.... There is no favorite way. SolidWorks is awesome because there are many techniques that can be used based on one's needs. All opinions here are valid workflows for each respective user and I am sure they all can state very concise reasons for doing what they do.
Know the software well and learn the many techniques and workflows that are possible to get the job done. Choose the best approach for your given situation.
FWIW....
This always gets me riled, I shouldn't even post, but I'm going to anyway. If you work alone or with just a couple others and you're designing one offs, tooling, custom order one-time-build machines, etc. you have the luxury of whatever method you like. You can listen to the evangelical CAD leaders and trial and error methods while getting actual work done because if it doesn't turn out to be an improvement there's no long lasting issues, those files are never seen again anyway.
Some of us are in a world where external constraints find a way (usually indirectly and learned too late) of defining how you will model. The users go to training or conventions or look up online how to do something and someone is raving about how easy a certain method or process is but there is no use context provided. So the users start using those methods that we as a group have previously ruled out as beneficial workflows and muck things up again. But it's not just that one file, not even all the assemblies going up the tree, add to it all the files that were created by copying the original to a new part number then edited. I'll try to explain a context where that I find exploring new processes on actual product can cost a company tens of thousands of dollars.
edit: I whole heartedly believe the "evangelicals" mean no harm and really just want to see other users be most efficient at using their beloved CAD system.
So, top down is not much help because the top already usually exists. Sometimes I do "middle down" for new sub assembly but all links must be broken, all sketches defined. Why? You ask. Multiple where used, then down the road, the original parent get obsoleted and no longer maintained, now what? Reference nightmare. Each part file must be fully self defining, only exception are mirrored parts or a part that is made from another part, but those are still a one way parent-child relationship.
I do like using animated sketches very much. Can lay out a mechanism with great efficiency in digital 2D. Using lines as force vectors where the length is a ratio of force is very handy.
I do like "skeleton sketches" not sure what to call it, within the part. I'll make two or three or even four sketches before the first solid feature. I define the mounting points, usually bolt holes, in sketches with no closed profile. This keeps the sketches simple and feature tree clean. Then I drive my later sketches that define solid body features from the first so that no mater how I move the bolt pattern or hole diameter my part has x.x" from the edge or the hole or whatever. This allows transparency of design intent (connect these other parts with these holes or mounting faces) as well as quick editing from the parameters table later on. Often not even opening a sketch to adjust the parts. The minutia of how these inter sketch relations and dimensions are setup seems to be CAD dependent though and I'm not in an impressive part of the Solidworks learning curve yet.
My $0.02
Everything is based off of Sub-Assemblies - every part is defined in an assembly, is it top level assembly or a sub-assembly, (unless it is a interchangeable component).
I only use top-down-save-bodies when I am actively seeking trouble.