Configurations vs Family of Parts
This is a topic I want to open up to discussion from both sides of the aisle here, but in particular I’d like to hear from the Edgers. I see the theoretical advantages and disadvantages of the concept of “configurations” in SolidWorks, where many versions of a part can be stored within a single file. I’d like to hear about the advantages and disadvantages of the Solid Edge method for Family of Parts.
Just for clarification, let me go through the SolidWorks configuration idea for those who aren’t familiar. “Configurations” in SolidWorks are basically versions of the part or assembly where you can turn on or off features, change dimensions, colors, certain feature options, and other similar kinds of things in assemblies. The configured part or assembly remains a single file, and there is a list of configurations, allowing you to switch between the configs, and even switch which config is used in an assembly or external reference. Configurations can be driven several ways in SolidWorks:
- no organization, just features turned on/off and dimensions changed in various configs
- tables for individual features
- tables for parts
- Excel spreadsheets that control variables/dimensions/properties
You can use configurations for various purposes in SW:
- to simplify parts/assemblies
- to show size variations of parts/assemblies
- to show variations with different features/parts
- to temporarily eliminate certain features you may want back later
- to show assemblies in different positions
- to show parts with secondary operations such as machined castings, or plastic parts with pressed inserts
- to show parts in a flexed state, such as a flattened o-ring, or a tire under load
Actual applications include:
- an entire family of screws might be configured so that all sizes of SHCS might be found in a single file
- simplified versions of a part or assembly that have complex features removed to make it easier to work on them
- versions of an assembly shown in different positions
This is an oversimplification of configurations in SW, there are a lot of different configurable items and just as many uses for configurations. Configurations are a widely embraced method in SolidWorks. There is no question that they are useful.
But on the other hand, a lot of users have been bitten by configurations, and actually prefer to use the Solid Edge Family of Parts type method within SolidWorks – they save each version out as a separate file. Probably the biggest example of the failure of configurations is SolidWorks Toolbox. Because files of the same name can have different configurations, moving assemblies between different Toolbox implementations can result in a complete loss of fasteners from an assembly. Toolbox can be set up to use configurations or separate files. The only safe way to use it is with separate files.
Several drawbacks exist when using configurations:
- not all PDM programs can track individual configs
- if you delete something, it is deleted from all configs
- if you don’t use a table or Excel, managing configs can be messy
- files with many configs can become huge
- switching between configs can be slow
- managing nested configs can get confusing
- believe it or not, there are bugs that might make some aspects of configurations unpredictable
- Toolbox configurations automate big problems
Given the Toolbox argument which has raged for over a decade, it is easy to see one reason why Solid Edge users might prefer to use the separate file approach, but having used configs within a single file, it might seem limiting to not be able to turn on or off collected features within a part.
I wasn’t able to find any good demos of Family of Parts in SE on Youtube, or even anything particularly helpful in the SE Help. Even with the Command Finder I wasn’t able to locate the Family of Parts icon to get started. I don’t think there’s a very good conceptual overview, or a workflow overview of this functionality, so this is one place where Edgers can step in and fill in some of the practical details that the documentation has left out.
Edgers, what do you think of the current state of Family of Parts? Is there anything missing or anything that you think works great? If you’re familiar with SW, can you compare FOP/FOA to configs?
I have been reading with interest about FOP compared to SW configurations. It is clear to me that SW has a better idea here. All catalogs that I have of standard parts tabulate with the part number, dimensions and specifications in a row. In many cases subsequent part numbers have a change in one or two dimensions that proceed in steps. For instance AN fasteners are available in lenghts in steps of 1/16 inch. So a simple formula and fill down can be used to generate dozens of configurations. I think that it is better to have all configurations in one file. The SW toolbox is kind of nice, but the parts are never quite correct and do not have the part numbers that I can order. I do not use it anymore.
SW files are all pigs about 1000X oversize compared th the information that I enter to create them. SE files seem somewhat smaller, but still pigs. I will begin to say nice things when SE files are 1/10 the size of SW. That would make them only 100X piglets.
I have been a SW user for a long time and have been using SE for over a year now. At wiese europe we use a lot of parts wich are the same in shape but not in material.
So we tried to make a Fop but could not find a way to put the material in the table, also we use alpha numeric part numbers and there was no way to put those in either, only numeric values allowed.
In a second example we tried to put in excell base tables in the Fom, but the if then expression was not configurable.
The third issue we experienced was: if you use a family an the configuration at the same time (welded-assembled) in the 3d enviroment it all works fine . But is you make a drawing and superinpose the two members it dous not work any more. It stores only the grafic information of the last saved configuration member and forgets all others.
Thats why we don’t use it , it does not work in SE
In SW on the other hand we have no problems to do this
We even mentioned this to the helpdesk and they even told us not to use it like that becouse it dous not work.
Sammy
Dan,
You wrote:
“What we call “Family of Assemblies” is single file for all members and “Family of Parts” is multiple files — one per member.”
It’s seems kind of weird to use different priciples for parts and assys.
Any idéa why SE choosed to do so?
Advantages?
I have some questions about assemblies.
Is it posssible to create several configurations in an assembly
using different configurations of parts (FOP members)?
Is it posssible to create several configurations in an assembly
using different different configurations of sub-assemblies?
How do you control which configuration of an assy to be used?
BR/Chris
The reason they are different is just historical in how/when they were developed. We’ve talked many times about choosing one horse or the other, but since neither horse seems to vastly outrun the other, we have opted to not invest to change it.
In regards to your questions, yes you can make FOA of FOP and you can make an FOA that includes other FOAs.
Hi,
Here is a video about your questions:
http://www.youtube.com/watch?v=cW3bMZef2LE
BR,
Imics
Hi,
I’m a SW user since 1998 but at the moment I’m working for a company using Inventor. I have used Inventor for 18 months now and it’s a pain. It’s user-hostile, tedious and unstable POS. It’s amazing that Autodesk are able to get paid for such a poor product. I would not use it even if it was for free.
I’m trying to convince the company to get rid of Inventor.
Catia is to expensive.
Creo to complicated.
Some other alternatives like Alibre and IronCad are not really an alternative. So the real options are SW or SE.
SE has limited number of users but seem to be competent.
I was curious about how configurations (variants of parts and assys) works in SE. I searched and found this interesting discussion.
I was surprised to see that SE use separate files instead of storing the variant info in the same file.
IMHO the architecture with separate files for variants is bad.
Inventor use that architecture.
In Inventor variants of parts (iParts) are created in a mother-file and a new folder is created where copies of the file is stored. One copy for each variant/configuration.
It’s quite easy to create the part variants.
The mother-file is inserted into assys and you select wich variant to display/use. The extra copies are never touched by the user. They just exists. The variant can easily be switched.
One problem is that if a part is inserted into an assy as an normal part and then later converted to an iPart the part has to be replaced and all constrains/mates blows up. Typical Autodesk. No attention to details. Screw the user.
Apart from that iParts works great.
iAssemblies which are the name of configured assys has shown severe stabilty issues. As for iParts an extra folder with extra copies of the assy is saved. iAssys seem to slow down the computer. Loading and rebuilding takes much longer.
The extra copies in the extra folders creates problems.
The extra copies often remains checked out even if the mother file is checked in to the Vault.
Sometimes there is rebuild issues and cryptic error-messages.
Sometimes iAssys forgets wich version of iParts to use and I have had to repair the control table many times.
I have also seen iAssys with parts all over the screen.
I have iAssys tha cannot be opened at all without crashing.
(Seems to be fixed in Release 2014)
Common for both iParts and iAssys is that the separate copies of the files must be manually generated after changes to be sure instances used at higher level is updated and displayed correctly.
SW’s principle with all data in one file is nice.
Simplified file-management!
Poolproof principle!
SW configurations is extremely powerful and easy!
I agree that it’s not a good idéa to use configurations for screw sizes. It’s better to save a copy. Then mates/constrains will stay when replaced.
I also agree that SW toolbox or Inventors standard parts should not be used “as is”. Use the part generator and store the part with a good name in a good place. No problems!
There is not such a thing as the perfect cad-program.
SE is ahead of SW in some areas but I value the powerful configurations higher than Synchro-technology.
If I would pick 3D-tool today I would choose SW again.
/Chris
There is no doubt that SolidWorks Configurations are very well done. In general, kudos to whomever on their team conceived it and implemented it. In Solid Edge for various reasons, we are mixed. What we call “Family of Assemblies” is single file for all members and “Family of Parts” is multiple files — one per member. So we have great experience with the pluses and minuses of each! We variously debate which is better and the answer is NEITHER. They both have good and bad things about them.
The biggest downside to a single file for a family of parts is revision management and part number tracking. In general PDM and ERP systems don’t deal well with a single document which has many part numbers associated with it (each representing a different “real” part). Also, if you need to revise a single member you need write access to the master, which may not always be possible in a structured workflow.
Anyhow. good and bad, no matter where you look. I suggest you contact your local reseller partner and look closer at Edge. i am confident you will find more good than bad, when you look more deeply.
PS> in Solid Edge you NEVER place the master as a part in an assembly. you always place the member you want. It is easy to swap members when you want to because the master can be found via the member and it points to the other children. Placing the master is the root of all evil. Likely the issue you are experiencing in Inventor.
Best,
Hi Chrisinstockholm
Here is a video how FOP works in Solid Edge:
http://www.youtube.com/watch?v=TOocuZBCoQQ
Very, very reliable, you can handle them in PDM system (revision management), the file size is smaller than sw’s. You can define Alternate components…
BR,
Imics
FYI
http://www.youtube.com/watch?v=sBoCEFO7fO8
Uh, Chris. I notice your video got removed. I did get the chance to watch it. Looks nice. I was thinking it was a bit early to be hearing about that stuff. Anyway, we’ll wait.
Ah yes, this was a snafu. The launch video is supposed to come out following the launch! 🙂 at Solid Edge University. Some yahoo jumped the gun and pushed it to YouTube. It has been pulled down. Sorry for the confusion.
@nice presentation!
Does SolidEdge offer anything akin to DriveWorks?
Configurations are one of those things in SolidWorks that many use but don’t use properly. Or rather they use it but because the interface to it is so easy it is used without too much thought. Which is where apps like Driveworks come into play in that they force the user to be a bit more organised.
We do one contract for a customer linked to DriveWorks Xpress where we can alter a master assembly in minutes and update drawings. It is a genuine time saver.
Configurations are definitely one of the Solidworks crown jewels. It is one feature we use on almost every project. I find them very robust (but then I’ve used SW for 15 years).
BTW Matt you can delete things in configurations. Use the delete body feature then suppress the feature for the configuration.
Kevin,
Delete body does not delete anything at all. It just adds a feature. The body it supposedly “deletes” is still stored in the file, which you can prove by suppressing the delete. So it was never deleted.
There is no doubt configurations are misused.
Driveworks is very different from configurations. It’s more like SE’s FOA, having a separate assembly for every version.
Hi Matt
(After reading my reply, it seems that FOP is a bigger subject then what it is look like from a first look, hope I do not have post too much info, some info will might need to be review in a different context to better understand its concept.)
I believe many if not most of the CAD designer try to bring this down to a technical question. Part variation either Configuration or Family Of Part (FOP) is a not a technical question but a manage question…what you want to manage.
I do not know any CAD designer, OK maybe a group as small as a sample of start dust, which will wake up in the morning and will say….. Youpi I will manage part variation.
First let clarify few things (from my personal SE point of view that is not necessarily the official Siemens point of view)
to simplify parts/assemblies
You mention Configuration is use to simplify part/assembly, not sure this is the right application for this. The simplify version of a part is by my definition another way to display a part and we should not have multiple version of the simplify representation. For this reason SE make a clear distinction at the part and assembly level between the two concepts. We have a simplify mode for part (under tools) and the same in assembly (under tools). Also part simplification implies a different mathematical representation (see below).
to temporarily eliminate certain features you may want back later
Eliminate feature temporarily to have them back later???? OK this one is kind of obscure to me because when I place a feature in a part it is either something I need or a reference. A feature cannot exist and not-exist at the same time.
Again SE make the distinction by having a solid body and by using surface body as a reference, we use the visibility check box to show or not reference. If you create a solid feature and you play with its active/non-active state, that’s mean the topology of the part will change making it hard to manage at the assembly level. Especially if you desire to have inter-part associativity.
Just a quick note if the topology of the part change that’s mean the mathematical representation or definition change. This is something you do not want because the 3D kernel that track element index everything as a mathematic entry, change the mathematics you change the index reference….
to show parts in a flexed state, such as a flattened o-ring, or a tire under load
Not the same as the previous point but similar. This one is in a gray zone because it will depend how you will intent to use part variation to get the desire result. But if you play with feature on/off state you might not use it how it should. We need to accept that some of the feature/functionality is still out of range (…..for the moment future development in CAD software might remove this limitation). We can find workaround but in this case we cannot complaint about it.
As for the concept of flex, SE again makes the difference between rigid and Adjustable part (notice that adjustable is being use instead of flexible) you can find adjustable under Tools in the group Assistants. At the assembly level RMB and select from the contextual menu.
Family of screw
This one is my favorite it is almost like an urban legend and it show how lazy people are when it comes time to manage CAD documents. However I give them credit because 1st I also fall in this trap when I start my career 2nd CAD vendor (read here reseller) are so desperate to win account at all cost they will do anything to make their software look like the miracle of walking on water. So instead of educating their customers right from the beginning when they sell the software, they just blend different concepts to create a giant fireworks. And worst they still continue educating their users with false assumption.
The real name of a family of screw…drum roll……should be call standard parts……
to show assemblies in different positions
OK yes the same concept can be apply to assemblies but we need to keep in mind that if we apply a similar concept that does not mean it is identical and we cannot always reduce to the smallest common denominator. For that reason in SE we use the same concept at the assembly level, but we talk about Alternate assemblies. Alternates assemblies comes into two options Family Of Assemblies (FOA) and Alternate position.
to show size variations of parts/assemblies
to show variations with different features/parts
to temporarily eliminate certain features you may want back later
to show parts with secondary operations such as machined castings, or plastic parts with pressed inserts.
simplified versions of a part or assembly that have complex features removed to make it easier to work on them
versions of an assembly shown in different positions
All the above will fall under what I call good reasons to use FOP/FOA
Part/assembly variation, no matter the software, if it is use with the wrong intention, it will create more harm than the good we expect from this tool. But at the same time the software should help you by not trying to merge everything in a single feature/command/concept.
I repeat myself with different words, it is a tool not an obligation or a goal we need to achieve. Part/assembly variation will not reduce or simplify parts/assemblies management. On the opposite it will add a layer on top of your CAD duties.
Toolbox
SW Toolbox was mention. Again SE makes the distinction between FOP and what we call Standard parts library. I personally never place a FOP in the standard part because it simply does not make sense from my point of view. The standard parts is the tool if you want to manage and use a family of screw
So as you can see SE keep separate all the workflow or at least understand that different concept exist and need to be apply with small variation base on the usage we intent to make. Some can be mix but it is not recommend if you want to keep a minimum of control.
OK enough of my esoteric speech and let’s talk about more technical stuff. So instead of just saying what I think it is, I will try to describe/explain.
http://www.solideadn.com/SEHelp/ST4/EN/famprt1a.htm
FOP can be seen like a family tree, you start with an individual, which can have as many children as you want and each of those children can also have as many children which in turn can have children and so on.
You can manage your FOP from two locations a basic panel or a more complete tool name FOP Edit Table (to help clarify SE does not rely on Excel to manage FOP. We have a standalone table inside SE part. OK I know SW people are probably convince that Excel is the only way of doing things what I can… it is not 🙂 )
The part that contain the FOP information, is call the master. It is not recommend using the master part in an assembly in production. With may be a small variation where you have and assembly template that you clone, Right after you clone it, you will replace the master by one of its member.
Each member defines in the FOP table need to be published in order to be use. This means each member will have its own private space.
Once the member of the FOP table are populate, Solid Edge will regroup this family at the assembly level into what we call “Alternate components” A tool that allow users to switch between members of the FOP.
In the FOP table:
• You can create, copy, rename FOP member
• Delete members, delete a member does not delete the part, just the definition in the table. The member will still remember where the parent is even if the entry is deleting from the table. You can break the link definitely if you break it at the part level. You can re-establish the link by recreate an entry in the table having the same name.
• Feature can be supress or unspress
• Live Rules can be ON or OFF
• Each dimension can be control individually for each member
• At any point in time, you can access the master from the contextual menu of any FOP member.
• From the master you can open any FOP member
• From the master you can update any member ( just be careful if the member is used in production and you change its mathematical definition)
• Opening the master inside Revision manager will give you the first level of the FOP.
• Propagation is by default one way parent to Children, but since each member are individual file, you can establish link between them. However consanguine union in the same family may lead to weird children. From a management point of view you run after trouble, but if you are willing to do so, do it but do not complain 🙂
Rules of thumb draw the relation three on paper and see if it makes sense. If you have multiple level of children make sure the information is propagate. Because if you have three level and level two is never open, no information will reach the third one. No mystery here just plain logic.
The problem is that configuration can’t be managed under PDM.
Configuration are under the same file , then the file is writable or read-only.
Different configurations can’t have different revision or state.
If they have, it is a workaround, compiling an attribute in the configuration.
FOP is the best solution for lots of dimensions like unified standard screws.
For less configuration, SolidWorks idea is useful.
I am most excited to learn more about SE. I find table driven configurations to be a very powerful tool in Solidworks. It can bite in strange ways when I try to improve the model and replace the configured part with the improved configured part in an assembly. The sizes get all mixed up and may not mate correctly. I am drifting away from the toolbox as the parts do not have conformity with what I buy. Every standard part needs to have good geometry, and full part number and sourcing information. I am now mostly using my own library of standard parts. A file for every screw is not a big deal the problem is that solidworks files are pigs 1000X larger than necessary.
How is the file size for SE parts compared to SW?
Does SE have a nice standard thread feature?
Can SE features be neatly arranged in folders within folders in the feature tree?
Hi,
Here are two videos how FOP works in SE.
Traditional mode:
http://www.youtube.com/watch?v=TOocuZBCoQQ
Synchronous mode:
http://www.youtube.com/watch?v=ZOnf_UZ88yg
SE file size is smaller than SW’s because SE creates individual parts from master (the name of the process is populate).
If you change a diameter which has thread then SE will look up the new thread size from thread database (look at the first video).
You can make groups in the feature tree if you need for it (I love this in synch too).
Regards,
Imics
In my opinion configurations within a part in SWX are a very useful tool because it allows me to have various states of a part. As an example ‘as molded’, ‘for FEA”, “for drawing”, as machined etc.
I do not have a lot of good to say about toolbox. I worked on a large project last year where assemblies had to be shared between different companies with different toolboxes and it was nothing short of a disaster.
I completely agree with Peter McKay’s comments at the top. If I need a fastener, washer or ball bearing I do not like to use configurations. I create the part I need and save it as it’s own part. Over the years I have built up a library that has proven to be very adequate for the work I typically do. Like Peter says, I typically end up using the same sizes over and over, so there’s really not that many different parts in my library.
Hi Matt,
In SW the way I used configurations that was robust enough and a real time-saver was when working on an assembly with various number of parts.
Like when I worked on a above-the-ground pool. They are available in several diameters and they all use the same parts, only in different quantities. With an Excel spreadsheet it was easy to control the parameters and check that all the parts were functioning for the different pool sizes. Was also great to generate BOMs for the different sizes.
It was a lot more tricky with parts configs, like when the parts had two sizes (two pool heights for example). There was always the risk of doing a change in one config that would break the other configs then break some links then break the assembly then break you weekend plans.
I would like to know if SE has some provisions for config-like functionality in assembly to manage product options.
Marc
In Solid Edge, we have separate concepts for Family of Parts (FOP) and Family of Assemblies (FOA). You would use FOA to do what you did with the pools and the part counts. (you can also have an FOA that uses FOPs).
Hello Marc,
Attached are two examples of Family of Assemblies (FOA). The one is a 16 row 3ft maize planter frame and the other a 16 row 2.5ft frame. They are all from the same assembly file, just different members. If you look closely at the pathfinder you will see that they use different options (wings and center frames) from the groups that I have created. Some parts are shared between members (for example the “VACUUM CAPPING PROFILES”) but can have different positions and relationships. Creating all these members can become a bit tedious but it is pretty robust.
Regards,
Theodore
Matt
In terms of getting help using FOP, go to “Tutorials” on the SE opening screen and you will find one for FOP which does a pretty good job of expalining how to use it.
I work a couple of days a week in a SW design office so I get to see a fair bit of SW. The first thing that struck me about SW configurations is how quick and easy it was to set up – really nice interface and very intuitive. The second was that in this office, they had decided that configurations should not be used on final production models (only R&D development) as they were simply not sufficently reliable (they use PDM). I experienced this just 2 weeks ago (this was not the first) when we opened an assembly and part of it was missing – turned out to be a part with configurations.
SE FOPs are slow and clunky to set up in comparison and the interface is not intuitive. Also, it produces a part for each configuration and this is less “neat” than the SW implementation. However, it is very robust and I have no hesitation using it in production models.
For me, the SW configs score during the development of a design as it is fast and flexible. SE FOP scores for an established design that you want to set up with different options and need rock solid reliability.
If SE FOP had a much more user friendly interface and transparent workflow then I believe this would be the superior tool. My guess is FOP is an underused functionality in SE because of these short comings.
Roger
Ok so I decide to make a FOP – A,B,C. Does that mean with the nature of direct edit and live rules changes wont propagate to another family member or is there a sort of history/association in there? For example if A is a simple part with a circular hole and the hole is a different size for B and C can I move the hole location on any of them and have them all move or do I have to edit each one or is it ordered from a parent? can I change which is the parent later? can I make rules between the children I choose so that a hole on C is twice the diameter on B but not related to A? Sorry if these are silly questions. I guess if I saw a demo of it in action that would be better. 😉
Ok so I decide to make a FOP – A,B,C. Does that mean with the nature of direct edit and live rules changes wont propagate to another family member or is there a sort of history/association in there?
The parent can be either ordered, sync or hybrid but the child is always ordered, so yes changes do propogate.
can I change which is the parent later?
Pretty certain the answer is no.
It is also possible to convert the child to sync and continue working with it from that point as an unlinked part.
Neil
“..can I move the hole location on any of them and have them all move..”
Yes, with a small variation…
open the master from any FOP member, do what ever you have to do.
Publish the modification.
I’m coming with a more complete explanation.
Forget to mention, if a modification happen while a part is offline (close). on the next open
I recommend to keep option one to have the control and keep the warning.
Matt any restriction on the length of a reply?
OK then looking at the big picture it seems SE is rather more bound by order than I might have imagined from the direct edit publicity. Is that because it is still a work in progress or is this how it is by choice for machinery stuff or because of some inherant limitation? I think ID people might appreciate still more flexibility if it could be managed. FOP seems like it is not quite all it could be like those pierced curves Matt tried to drag and that didnt quite pan out as we might have thought/liked. Perhaps it is because no one has really tried to use the flexibility in a demanding or imaginative way before? Maybe SW users have a different perpective/experience to bring from configs to FOP that can benefit everyone.
Neil
“…OK then looking at the big picture it seems SE is rather more bound by order than I might have imagined from the direct edit publicity…
I’m curious why you got this feeling of being bound by order (design)? Seeing you talking about ID, i have the feeling that you are closer to produce artistic design then mechanical/calculated engineer design . Do i get this impression wrong?
“…Is that because it is still a work in progress …”
From my perspective CAD software are work in progress since the 50’s
“…or is this how it is by choice for machinery stuff or because of some inherant limitation?…”
Machine design is a strong part of the design philosophy. Do SE want to limit to this, I’m not sure remember when they introduce BlueSurf and BlueDot, those tools can still today be used to produce nice design and product.
and now Synchronous from my point of view ground have been layout to lift more limitations then before and push the boundaries of design. Now the question which direction the SE community want to push SE….
Not sure i understand fully what you are saying. The topic is FOP and your comment seem oriented to part design (ID). “…. FOP seems like it is not quite all it could be like those pierced curves Matt tried to drag and that didn’t quite pan out as we might have thought/liked….”
I have the feeling that Matt have some answer about the splines and the pierce point in Sychronous sketch. Also remember SE is not only about Synch it is also about mixing it with Ordered design where you can use BlueSurf and BlueDot.. Could we have more of course. Now the question is how much are you really limited with the current tools available today (or in a month ST5)?
Here a video where i import a dumb part recreate the surface, add more control curves and use BlueDot to manipulate the surface.
http://www.youtube.com/watch?v=JOryQdsq71Y
I also made an attempt 3 years ago
https://vimeo.com/3331350
And i let my self go on this one
https://vimeo.com/1725889
Back to FOP
..”Perhaps it is because no one has really tried to use the flexibility in a demanding or imaginative way before? …”
Links can be establish between publish member of a FOP. And I’m sure we can push the imaginative way in uncharted territory ( ask Dan I’m sure he will have few anecdote about some of my imaginative request :-)) But again this goes back to how much are you willing to manage?
The problem when establishing links is when do we reach the too much links limits. We deal with the human factor too much links and the brain will short circuit. So questions we should ask do we give the ultimate freedom to give a rope to user ( create unrecoverable damage) or do we simply give them enough freedom so they only paint them self in the corner (no permanent damage that can’t be undo or correct just time consuming) or do we try to protect the user form it own mistake? This is a delicate balance hard to obtain.
OK like i used to say, let start with this and see where it goes…
Yes my main interest is ID stuff so I am definitely interested to know how SE can handle the equivalent of SW configurations ie FOP. Sometimes you want to make size, layout or styling variations for instance. In the extreme if the tools are flexible enough you might try to use it to explore concepts rather than produce sketches… I am curious as to why you think the topic being FOP means somehow it is not applicable to ID. There is alot more to ID than pulling around the odd surface. Perhaps it is a gulf of awareness between disciplines or just a different focus. I wonder then as an accomplished SE user how you would view a small ID invasion into SE? Is this good or bad? How far would you like to see future directions of SE influenced by SW refugees?
Neil
“…Sometimes you want to make size, layout or styling variations for instance….”
Having different size…. that’s no problem
Layout….. if you plan correctly you master and the propagation of the new features you want to test, that should cause no big problem
For styling,… since each body are in different file you can apply them without problem. You can even propagate the color from the master to the children and repaint only the section of the children that need to be tweak.
“….if the tools are flexible enough you might try to use it to explore concepts rather than produce sketches…”
Not sure about this because not sure what concept versus produce sketches means/involves exactly. Please provide more details.
Have you take a quick look a the video i post where i modify and import part. The same could have been done using FOP. Perhaps we should look at a workflow that will involve mixing FOP and Part copy. Will you be able to attend the ST5 launch?
“… I am curious as to why you think the topic being FOP means somehow it is not applicable to ID…”
Maybe i should have say that FOP what not design initially for this, but after all may be it can do more then what is was design initially. So far i think we answer many of your request except the reverse direction between the master and the child.
“…. I wonder then as an accomplished SE user how you would view a small ID invasion into SE? Is this good or bad? How far would you like to see future directions of SE influenced by SW refugees?…”
ID invasion inside SE would be just perfect. How far i would like it to go….as far as your imagination and needs can be answer.
I have FOP (Family of Parts) in SE for fastener families in the past, but do not recommend it. Instead I prefer to have a single file for a single bolt and save a copy and modify it for when I need a different size. My experience has been that whilst you would think something like a bolt or screw would never really change and could be locked down, inevitably things evolve. This could be you modelling method, new features in the software, or different metadata conventions.
My experience has also been that of all the possible fastener sizes, you only ever use a few, so creating a new one each time might seem tedious, but the reality is that it is not. In my experience…
Having hundreds (sometimes, but often tens) of versions controlled by a single file makes changing these things a massive job.
Secondly, if you have a single parent part, with multiple child parts, you are creating a lot of links. These links are “Insert Part Copy” links which are very robust, but they are still links that can be broken, or take forever to search through and update when revising or updating files.
For other applications, for example a storage rack that might hold 1, 2, or 3 bottles, FOP is very useful and a time saver.
Peter.
I’m with you Peter. I create a library of common use parts and bring copies in. I don’t have anything like Insight set up but even if I did my parts have to be able to travel with me without being dependent upon a server connection or parts library on another PC. I quickly decided that the dependencies created with links were more of a headache than saving each part out as it’s own part.