The way you are doing it by mating everything to the fixed component is the correct way. If you did it the other way if you change something in a component that would alter where the mate is then you would have to go and change the mate as well. That would be a nightmare on a big assembly. If you have it mated to another part then mate would still be correct after.
Just my two cents!!
exactly my point ha-ha. It feels like they are just trying to find a way of modifying a component without fixing the assembly afterwards.
I don't know that it's the worst idea I ever heard, but I certainly wouldn't recommend it. I do have one or two suggestions that may help.
1. I don't know how much you use patterns in assemblies, but I've learned the hard way not to mate to parts brought in with a pattern unless it's absolutely necessary. Doing that is just about guaranteed to cause stability issues.
2. Try not to stack too many mates. For example, mating Part B to Part A, then mating Part C to Part B, then D to C, etc.
3. While I'd agree that mating everything to the 3 primary planes would often not work, I would suggest mating as much as practical to the them, other planes that are independent of any part, or to sketch geometry within the assembly instead of to other parts.
4. Use sub-assemblies whenever it's practical.
This is good stuff! but I want to make sure that I understand your pattern comment.
are you saying that I shouldn't use a feature driven pattern on a hole wizard when it comes to fasteners?
our company doesn't have a modeling standard and that is what I am working and a big thing that I was taught was to use the whole wizard.
No, using the Feature Component pattern is fine, along with any other kind of Pattern. I use them myself. I'll try to explain better.
Assume you bring in a Part A and fully mate it. Now you create a Linear Pattern (or Circular Pattern, etc.) of two more instances of Part A, which I'll call A1 and A2. Then you bring in Part B. When you're mating Part B, you should be able to mate it to Part A without any problems, but don't mate it to either Part A1 or A2 if you can avoid it.
ok that make more sense thank you!
Not that it would be the correct way for your company, but as a major example, the auto industry does exactly that. I really think it is all what you are looking to use as your inputs and what your requirements are. If the person(s) suggesting the idea are really invested, I would say to them that they should create an existing assembly from scratch using the method they want and see how easy it is to make typical changes you guys make. Run it through it's paces and see what shakes out.
When I build assemblies I do as you said: insert the first component as a "base" component. Make sure it is fixed properly to the assembly origin and/or planes. After the initial component insertion, I then insert the other components and mate them to the planes and/or axes of the assembly. At times parts may need to be mated to other parts; however, I try to mate as much as possible to the base component and the assembly's planes and axes.
You are correct that the model assembly would no longer be parametric. I am not sure what stability would be obtained by building an assembly this way. In the old days of Auto Cad there was no "constraints", you just place and or rotate the part origin in reference to the assembly origin. I suppose there may be an instance when doing it this way may be beneficial. With today's fully parametric cad modeling software this is just a senseless approach. It would only lead to manufacturing mistakes down the road as well as drive the people crazy that have to update the assembly.
You could tell them they could eliminate this stability problem all together by hiring fifty draftsman, drafting tables and triangles. Also don't forget the vellum, diazo machine and drafting pencils!
I have had more issues with assembly stability then I can count. Some I inherited and some I created.
What has worked best for me is to assemble things to parts during the design stage - use the base and build off that, but before I 'release' it or let anyone else have access to it, I change the mates of the components to link them to assembly features, plane offsets and angles mostly. It slows me down initially, but I do it to eliminate the stability problem.
I worked with a person who would create a part model with nothing but planes and axis, use that for the first part in the assembly and attach everything to those features.
I am a big fan of parametric modeling, but if your company does not have a rigid and effective modeling standard, it has been my experience that you will have more trouble with parametric modeling than benefits - especially if multiple people work on an assembly.
We do a combination of some of the methods that have been described already. In our lower level sub-assemblies and parts, we relate the components/features to their particular origin. Then in our mid and upper level assemblies we have been using a separate "skeleton" component that uses planes/axis/sketches to define the locations of important features. The lower level assemblies and parts can then be mated to these features to fully define the top level assembly. It's a difficult concept for some of us to grasp initially, but seems to be very powerful once we get the hang of it.
When I started at my company, we had severe issues with model stability. With experimentation and practice, we have discovered that we need to use a hybrid of mating to the assembly origin and mating to other components. As always, our first component is mated to the assembly planes. The nature of our designs make it best for us to insert many of the components tied to one or two of the assembly planes, and to tie the remaining degrees of freedom to components as necessary. To support this functionality, we are very aware of the correct orrientation for Top, Front, and Right for every component. We choose where to put the primary sketches based on the required assembly structure for each part.
The nature of our products has allowed the use of weldments and sheet metal parts for most of our components. In many of these situations, it works best for us to tie to sketch elements rather than faces with our mates. I'm sure others have had very negative experiences with this, but it works very well for us.
As has been suggested by others in this thread, I would look at what features you need to have parametric ties with, and what remains static between your reuse of models. In my experience, anything that remains static should be tied to the most stable feature possible, such as an assembly plane rather than a component face.
I am interested in other peoples experiences as well in the hopes that we can improve our process to be easier and faster.
I agree with mating the planes and axis's, depending on the assembly and depending on how particular parts relate in other assemblies.
It is much easier to find a named plane and reuse in as you go. Like Center plane Front--Center plane Side and so on.
I always rename my planes as well.
Hum, I never thought how valuable it would be to name your AXIS? haha
Kathy Navarrete wrote:
Hum, I never thought how valuable it would be to name your AXIS? haha
My assembly template is set up with three named axes, one at the intersection of each of the three primary planes. I use them for the direction when creating a linear pattern. They're hidden so they don't clutter up the graphics area, but when needed I can select them from the tree, no need to make them visible first. This works much better than using the edge of a part, since if the part is deleted or edited you can (will) lose the linear pattern's reference.
I always create a axis at the intersection of 2 of the start planes anytime I am making a cylindricalpart or doing any revolve feature. Like Glenn said, this way you never have to worry about it moving or getting deleted why you change other stuff, like a edge can. Another trick is to link things to the origin specifically instead of letting auto mates happen. The origin never moves, but when you put a bolt circle, point, or line end point into a sketch and it references geometry in other sketches it can cause problems when things get changed in those sketches. I think this is why some people have mate issues when adjusting parts in an assembly.
Like with most things it all depends.
Sometimes the process of modeling a component can be simplified if one encodes that component's position within next level sub by way of referencing the origin planes.
And if done right, things can be modified and the assembly would update logically.
The point is it's merely a technique that can be used when the benefits outweigh the cost. The cost being that it may take some folks longer to lay this approach out and that others may not be able to interpret the modeling approach and could corrupt it to the point it no longer works.
The question i would ask anyone who thought the approach was totally invalid would be, what is their rationale for assigning the origin of any part? Generally i like to assign the origin around something significant like the product i am handling or some commonality among features. That seems like a no brainer, especially if you were going to put some reference geometry in there afterward anyway.
I use a combination of both practices. It depends on the job and how interdependent the geometries are.
Mostly i try to respect the origin planes at the subassembly level so that i can mate my subassemblies quickly about the origin at the next level assembly.
But to have all parts modeled around the top level assembly origin....that's a huge time waster for zero benefit.
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I think the worst part about that idea is that when you are modeling a component you have to know ahead of time exactly where in space it will be located in the assembly. This is practically impossible if you are working on a new design for something. The second worst part about that idea, as others have mentioned, is that if a part changes, say you change a hole pattern, the position of the other parts, like screws, won't update with the change. And it's not like you would just need to move them to the new place. Instead, you have to REMODEL the screw so that it's new origin is at the new location!!! I think I agree with you that this method of mating is the worst possible method and I would never EVER recommend it. I think the time it takes to remodel every component whenever something changes is going to be way more than the time it takes to just fix messed up mates.
If they are dead set on not keeping mates, then another option would be to model parts around their own origin as normal, then in the assembly position everything with mates, then suppress or delete all of the mates an fix everything. This accomplishes the same thing as mating everything to the assembly origin except you don't have to be psychic when you model the parts and know where they will end up, and also if you need to move a component you don't need to remodel it, you just need to float it, mate it, delete the mate, then fix it.
Oh I also forgot to mention that if a component is used multiple times, then mating to the origin would require different files (or at least different configurations) for each instance of that component. This is another significant drawback.
I am with you on all of that. I don't really like the fact that you would mate everything then delete it and fix it but it is a good compromise that I could live with. thank you for your input.
Dealing with "fixed" components in an assembly is a big pain too. We've had to deal with some of this and it's very difficult to deal with when you need to go back to make changes/updates.
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My company has had the same conversation. Personally, I am against it, but others have used it successfully. It really depends on your product. If it is well very defined and not likely to change, it can be quick and easy to add/remove options. Each option is a sub-assembly and you simply replace the sub-assembly for a new option. It also makes it super simple to automate assembly creation. However, as others have said, if anything major changes you are in for a lot of work. Constancy is key.
I prefer parametric mates. As others have said, build a base including planes and axis and mate everything off of that. In my experience, mating to planes/axis is much more stable than faces, lines etc. Also, never mating to a pattern instance if you can help it and use sub-assemblies. If you can keep these concepts in mind from the start, parametric modeling can be very powerful.
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We did it this way at a previous employer. We custom designed shag trucks and were using Inventor. The product was structured by modules. The top level assembly (finished product) BOM was a list of lower BOM's. Such as: body, frame, heating and air conditioning system, engine, transmission, etc. Certain BOM's were designed to work together. When a customer would order a truck, they would specify length of frame, single or double size cab, engine, wheels, etc. We would then open a new assembly and insert the specified BOM's by their alpha numeric number and mate to the assembly origin and assembly planes. Once all the BOM's were inserted, we could look the assembly over for fit. If things didn't fit, we would sometimes try a similar module BOM that would fit better, or have to create a new module BOM for that customer. The drawback is that we had a large database of module BOM's and would obsolete ones that weren't used after a number of years.
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You don't have to delete mates to fix things. Just fix them and the mates automatically go suppressed. If you need to update just float everything and the mates will resolve. There are some definite do's and dont's re maintaining stability. I find more subassemblies versus fewer is a big key. Subs seem to get treated like parts in the next level assembly; at least if they're rigid. People avoid subs because they don't understand promote. Avoid patterns generally, and as soon as you are able to dissolve the pattern, do it....much quicker. Try and analyze and repair all imported geometry. I find since imports are not native they mess with mate orientation...flip flopping around. Use limit mates sparingly and define after development of a motion. And as was stated several times before, don't daisy chain mates.
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That is the worst and the most damaging thing you can do to an assembly. I work with 1000's of PDM-Works parts and 1000's of toolbox parts and well as external non-revision managed fasteners (in our own library).
You should mate all the parts in an assembly to the "base" fixed part.
Once in a blue moon you will have a mating error when opening and assembly, because a part has been changed or relocated without properly opening the main-primary-base assembly. Sometimes people open just the sub-assembly to save time.... it happens... then the main assembly is screwed up without them knowing...
At least you would know that something changed and is not right.... imagine fixing everything to the origin and later on in production finding out that you have parts size or hole centering mismatches...
You're shooting yourself in the foot right there!
Fixing everything to the origin is very, very bad practice.
I woudln't like working with mates to only planes and axis, it would make it very hard to adjust things, especially in design phases of a project. I mostly will mate my first part to the 3 standard planes and then build from there. Over time, if your smart and use sub-assemblies properly then you can make a large assembly and not have many, if any stability issues. A few keys to this are:
1) Your first part in the assembly is your base part. Make sure it's tied down properly to the standard planes.
2) Use sub assemblies, especially where you have a bunch of components that are going to be repeated often. Using an pattern on a single sub-assembly is usually better than patterning 5 or 6 parts individually.
3) Try to uses mostly coincident / concentric mates, stay away from the more exotic mate types, and be ready to flip aligned / anti-aligned since a lot of times mate issues can be solved by changing this setting.
4) Get good at debugging assembly mate issues. It takes some practice to figure out what mate is actually broken when it's shows a long list of them in red. Usually one mate can be causing the issue and if you change the wrong one you can make it worse. Unfortunately getting good at this comes with practice.
I previously worked for a company that mated all the assemblies to planes in a master assembly. It was a very complex assembly and turned out to be a mess to work with. However, since the assemblies weren't mated by features it was not easy to catch the gaps in the part assemblies. You had to rely on the specific designer to be diligent with his changes and communicate clearly how they changed. In the long run it turned out to be disasasteres and cost the project long delays and money because when they went to assemble the assemblies they didn't align correctly.
Master assemblies do have their issues, and I would never recommend it for a complicated, one-off project. However, if you have an established product line and a proven master assembly, it can act as a skeleton to quickly build up a customized product from preexisting parts. Just my 2 cents.
What I've discovered is through the various classes, seminars, conferences, and years I've been using SolidWorks ... it's OK what ever way you choose to use the software. There's no "real" wrong way to do something.
At a previous company the VP of R&D tasked me creating a "Good CAD Modeling Practices" guide/document. I spoke with all of the other CAD guys to gather their input and I was just about to publish it when we hired a couple of new engineers. I thought it might be a good idea to get their opinion since they had been using SWx longer than I had. Boy was that an eye opener.
Long story short, we cancelled the guide because what might be good right now ... may not be appropriate later on. With different people's way of doing things and practices, advancements in the SWx software, etc. ... I think it's best to use the "parental philosophy" ... learn when to pick your fights.
But that's just my opinion.
It depends on where you are in the development cycle.
Early on, It is very helpful to mate plane to plane or from some odd feature. The example would be where you are trying differently shaped surfaces for covers for equipment. You don't need to finish out a molded part to get a feel for the design so the mechanical mates are not needed.
When you need to be exact in fits to components, that is where you go for the feature mates.
I almost always start with origin, plane and axis mates early in a design, especially when I am working with lots of complex surfaces.
I'll second Alex. I use 'default' placement for the first component and then after that I will use datums as much as possible over surface mates because they're much more stable features and far less likely to be modified or removed. When it makes sense I may do a complete assy based on default placements, this is usually when I'm making a top level assy that another group, with far less product knowledge, inside our company will use for manipulating via interchangeable configurations to make customer assys/prints.
Ahhh, the old "Top Down" vs. "Bottom Up" argument - or for us fogies: the Master Model approach.
Nice to see the frenzy translates across platforms.
I use Top Down whenever i have multiple plastic parts that need to fit together - I also use it when there is, for example, an optical path that drives the overall size and shape of the product. Especially useful when interpreting Industrial Design layouts.
This is for MAJOR components (housings, frames, etc...) The rest are assembled "normally" .
As many here have previously mentioned, it depends a lot on your company's specific product and design process. My company designs complete motorcycle vehicle assemblies from the ground up. With the complexity of our parts, often times completely surface modeled, it is very difficult to maintain mates, especially when a part makes it's rounds through several designers. We used to design everything around a common origin, which we referred to as bikespace. However, we would have issues with parts which would have to move as the design matures or components used in more than one vehicle assembly.
We are now switching to a coordinate system based approach which offers several huge advantages over the old method. A coordinate system can be updated where as the default origin cannot and you can have more than one coordinate system. Every component now has a coordinate system which coincides with the top level origin for each vehicle the part is used in. We have also added a special workflow to ePDM which allows a designer to check out a production released part to add reference geometry, specifically coordinate systems; the workflow verifies mass properties to ensure only reference geometry was added. It is the designers responsibility to verify that all coordinate sytems are up to date with any major rev.
This actually ended up giving us some great flexibility with our dynamic top level assemblies by driving the position of each component off a layout part containing coordinate systems for every moving system on the vehicle. This allows an assembly to be build where parts can move independantly of other parts to which they are sub assembled.
This is a newer methodology for us, but so far is turning out to work very well. We've tried building our assemblies they way we were all taught in school and ended up with nothing more than useless, unstable, bloated pigs of assemblies. And it's still always a struggle with new designers; we often have to let them crash and burn doing it "the way they've always done it" before they fully embrace our methodology. Again you have to experiment and find what works for your product.
In my previous CAD life, I used coordinate systems exclusively for surface model type designs.
I have been using the default origin in SolidWorks (I'm new), but will investigate SWX Csys's.
Personally, I have found that creating planes to be used for mating has made my life almost headache free. It does force a consistency in your naming convention, but everyone can then figure out how each component was assembled and easily identify each mate, while allowing for variability. Hope this might help.
I've used the Top-Down method a few times but I find you have to be careful at the beginning and as you go make sure your sketches are pretty well defined. If you build your parts in the assembly they'll all have the same origin by default (as long as you pick the same plane as the insert plane when you insert the new part). You get a bunch of virtual parts that you can save out later and that all carry the same origin and you don't have to mate anything because they are all just "In Place". Your parts will reference each other so when one changes all referencing parts change as well.
All the being said it can be a massive pain the in the neck. You have to make sure all your sketches are defined and have a pretty good idea of what's going to be effected when you make any changes. And when you go to make drawings of the parts you'll have to do a little more work to get the views you need. None of that is the end of the world but you gotta know what you're getting into.
Also Top-Down can limit you from reusing your parts in another assembly.
And as always, it depends on what you're doing and what outcome you want.
I would suspect this practice was developed by companies with large assembly files, common assembly builds, multiple cadd platforms, multiple users in the early days of CADD. I used to use it years ago with IGDS, VAX based, only because there were no surfaces/ faces to mate to. It is not wrong to want model in this method but with todays software and hardware it does not really apply. You need to ask yourself how much modification do I want to do. Verification of parts and assemblies will need to be manually checked and updated if necessary. Common part/ subassemblies may need configurations or separate files. Hardware could not be included in your assemblies. Advanced and mechanical mates would be eliminated.
My own opinion is you would be using your software for some old ideology that no longer applies.
This is a common topic
The disadvantage of having a base or first part of an assembly being a part in the actual assembly is that this part cannot be moved in the assembly .
Assemblies should generally start with a datum cone of your own design to suit your style at 0,0,0
Insert layout dwg if used
then insert main part - position and fix if req.
When building large assemblies uses axis and faces of other parts as 1st axis and plane in new part
cooperate with the system it is only unstable when you try something iffy
like hassles with editing pattern parts - BOM errors arising from multiple edits - and a few others
In The Automotive industry every component is created to a global position
when you create an assembly you call in the parts and they are automatically assembled into the position they would be on the car
this way you can create any sub-assembly and when it is used it will remain in the position in the car
this is very useful believe me
Normally, I start off with a fixed component. Use the most logical component to fix, i.e. the way that you would build it in real life.
Then add components, as you would build the assembly in real life, using the real life mates, i.e. screw mounting holes., flanges, mating faces, etc.
Kray, what kind of products does your company make?
The answer is simple: do what works!
Designing mechanisms likely requires that you mate parts to each other so that they can be articulated.
Style-heavy design often requires that parts share common surfaces and connecting features. Then it is advantageous to have everything with a common origin.
Automotive and electronics OEMs often use common origin modeling, so that parts can simply be dropped in and everything matches. Works well when work is spread out over a number of users and locations.
Of course, there are always minor exceptions. One would not want to anchor simple hardware in space.
Anyone who uses a phrase like "It MUST be this way because that's how I learned it" should be roundly ignored.
I agree, doing what works never fails.
And always try new things, because to Ronald's point the people who use the MUST phrase just never took the time to experiment and find a different way.
There is no one solution that works best for every scenario. There are, of course, best practices to observe, but which best practice is best depends on the design intent (or rather, "design for change") for your specific task. In general, the more parents a a feature has, the less reliable it is as a reference--which gives credence to the idea of mating to fixed origins. The stability hierarchy is as follows (excerpt from SolidWorks 2013 Bible, Matt Lombard):
- Assembly or part origin
- Assembly or part standard planes
- Reference geometry (plane, axis, point)
- Reference geometry from inserted parts (from using the Insert=>Part command)
- Sketch lines and midpoints
- Sketch endpoints
- Surface model faces
- Solid model faces
- Edges and vertex points
- In-context items
- Reference geometry
Notice that the most often used references--faces and edges--are the least stable. I find that a mixture of techniques is most suitable. For example, always have your "base part" fixed to the origin, with the part planes oriented the same as the assembly (to change the orientation, first orient your part normal to the face you want to be the Front Face, then select View, Set Current View As..., and select that face...note that any drawing views you have will be changed accordingly). From here, I like to mate subsequent parts in the same way they are physically mated--i.e. a fastener is mated concentrically/coincidentally to its hole and respective face, and then that fastener and face of the joining part is mated concentrically/ coincidentally with the assembly part to be joined. In this way, you will maintain an intuitive sense for troubleshooting any mate errors downstream.
Lastly, I think that modeling to a part origin makes more sense than building an assembly from the assembly origin. Of course, you will have to make sure your first sketch is oriented in with intent. Say, if you are making a plate with four asymmetric holes, your first sketch would be a square with its center point mated coincident with the part origin. This would allow you to dimension the asymmetrical features to their sketch origins in a predictable and robust way. This also facilitates the use of the AutoDimensioning feauture, which saves me a lot of time.
I would agree with Chase Nicole's suggestion. I worked on many very large assemblies and this is the best approach I found. You must first consider how are you going to deal with changes in the assemblies and parts. If the way you create a part is going to be hard to change, then rethink. The same goes for moving them in the assembly. I have fought with bad practices of mating or not mating completely and it can and will cause your assembly to blow apart if you mate to the wrong parts.
Parts should be created on a plane, not a distance from one. If that distance changes in the future it can cause a number of problems. Mating parts in the assembly is a much better way to handle this issue and can be changes much easier in the assembly.
What I found when mating is it is best to mate holes to holes first, then planes to planes or surfaces to surfaces. The advantage of mating planes to planes is if the surface or edges of a part is changed the mates will not be affected. I also found that if you mate everything to the first part it causes headaches there as well.
Sub-assemblies are a very useful tool. The more mates you use in an assembly, the more unstable the assembly is or more time it takes to open, work on, etc. They say the best assembly plan is to have 300 or less mating per assembly, therefore sub-assemblies with cut down that number.
The key thing to remember is what effect is being created by how you mate parts. If you move this part, what is going to be moved? Same goes for creating a part. How is this going to effect the assembly if you change it? Cause and effect is very important in your assemblies. So when creating parts, fully define the sketches when ever possible. Start with your base sketch, extrude, then add features.
Either technique is correct in correct design intent.
Advantages and disadvantages to each technique.
Either technique can maintain full parametric associativity when used correctly.
Of course, when using origin grounded components as the overall technique - the moving parts, sub-assemblies must have the usual DOF constraints.
In part creation I like the primary axi to bisect the part. For me this makes it easier to modify later on if needed. In an assembly I might not want the base component bisected as I normally need to reference a plane such as the floor or ground. So what I do in this case I mate the base component to the "Ground" Plane and then bisect the other two. Then the rest of the components are mated in accordance with how they will be put together (like a bolt hole or lined up to an edge, ect). This way I can utilize the parametric ability of the system to preview product modification changes.
I don't think there will be much if any performance or stability gain in creating a part in the way you are stating and mate it to the assembly plane. The mathematics involved in "mating" a component together is not really that intensive unless you have a bunch in there that you don't need and are creating a circular reference. What would be a better approach I think is if the main assembly is enormous then create dummy part's of sub assembly's to use in the main assembly for reference. For instance if I was modeling up an automobile I would create a single part of the dashboard and instruments instead of using the highly detailed sub assembly inside the main assembly. The dummy part can always be referenced in the engineering drawings to the corresponding detail assembly. However care must be taken that the assembly reference be updated if the detail is changed.
Here's something to think about:
When you build whatever the assembly is, are you connecting to planes and axis? No, you're connecting to faces and holes and studs, etc. Mate your assembly the way that it is going to be built. By doing this, you'll find interferences more easily. Also, should you change something on part A, which is mated to part B, you'll find out pretty quickly if you neglected to remember to change the hole positions, or stud lengths or whatever.
I worked somewhere that people were creating parts offset from the origin in order to be able to just drop it into an assembly and mate via the planes. I can't tell you the thousands of dollars in wasted time and material it cost us because something would end up being too long or too short or have slightly offset hole patterns.
The problem with the mate-as-built approach is that it is the opposite of what you need when you are trying to build matching faces and fastening features. Then you want the parts in-place.
Most of my projects are designed with major components in-place with common origins. All in-context work is done in a designated layout assembly. The layout is not the final product. The final product is built from zero with components that were defined in the layout, with mates.
As always, do what works for your situation.
Everything should be mated in your assembly the same way your parts will be fastened together on the floor. I've found may of screw holes in the wrong locations by doing it that way. If your mate fails, your part is wrong.
"Everything should be..." This is exactly the kind of thing to ignore.
There are many good reasons for in-place modelling. Done well, it can take a lot of time off of product development. (Remember "product"? That's what companies sell. Nobody sells CAD models.)
A big problem with mate-as-assembled in the development phase is it's very easy to lose the design context. Once that happens, it can take a lot of time to get everything placed back where it belongs.
For simple things, it probably doesn't matter.
As always, do what works.
"In Context Modeling" That's a whole new topic.
To continue "beating a dead horse" I am strongly in the camp of "it depends" and "each method has its place".
In my former job developing flight simulators many of our models were for developing image projection paths. In our case, we had a structure "over there" projecting imagery onto a screen "over here" with no physical connection between the two. In the field these same items were laid out with giant templates and anchored to the floor. My ONLY option was to mate to primary reference geometry.
More specifically, we developed a Datum part which contained only reference geometry. This one non-entity part was the driver for all the rest.
As far as using failed mates as a means of design checking - this too has its place. However, as the complexity of the assembly increases, the efficiency of the method decreases. For example, I use feature-based patterns as much as possible for fasteners. If you mate holes in two parts and then mate a fastener to that hole, there is no feedback to tell you the remain holes in that pattern are aligned. Also, the feature-based pattern for the remaining screws is only referencing one part with no feedback about mismatched holes. Ten bolts in a widget? No problem. 10,000? Whole different story. This is where tools like interference detection are woefully underused.
A primary tenant of large assembly best practices (to improve stability and load/rebuild time) is to locate parts with mates in preference over dimensions. Dimensions use significantly more processing resources to resolve. You want to minimize the total number of mates through efficient methodology and by driving as many into sub-assemblies as practical. You want to pattern as much as practical. And when you do create mates and patterns, reference them to the most primary of reference geometry practical (Origin, Front/Top/Right Planes, etc). As an example, if the face of Part A is parallel with a plane (front) and you need to mate Part B to be parallel with that face, it is generally a better choice to mate to the front plane of Part A instead of the face - but only if that corresponds to the design intent.
Again, if you have an assembly with part count in the dozens, the difference between methodologies will probably be unnoticeable - just a statistic in AssemblyXpert. If you have much larger part count and you have stability issues, these things need to be taken seriously. Since "practice makes perfect", start modeling as if every model will be part of a large assembly regardless of part count.
A blanket approach to model everything to the primary planes because instability permeates your models is a reactive fix-all. Make changes to your modeling methodology for the right reasons. Put together some training classes/documents that spell out good modeling stability techniques. Start sending the models back to the authors to be redone if poor techniques continue. Educate your users to think beyond the part they are designing. It does take some additional time - but WAY LESS time than fixing later, recovering from crashes, etc.
Yes, I know many of these statements fit into the category of "Motherhood and Apple Pie" - they sound good but Joe in the last cubical will NEVER change his ways. That is where the science of managing people comes to play... A topic for a completely different website.
- Laser optics sheet metal enclosure design using the Master Model/Top-Down modeling technique. All features are controlled by the master model. Each subsequent part uses the surfaces of the master model for final 3D detailing. Changes to the master model propagate automatically to the lower level parts ensuring perfect mating.