Top down design Layout sketches

I have been having a discussion about Top Down design and Layout sketches with a colleague, wondering what the group's opinions are?
Method 1 has the Layout sketches in the Assembly.
Method 2 has the Layout sketches in a Part, which is the first Part in the Assembly. That Part has only sketches and planes, no features.
What do you think is the best approach and why?
John Layne
www.solidengineering.co.nz
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Method 2 is by far the best. Master layout part for your asm and each sub asm should also have a layout as well.
..
On Oct 24, 5:10 pm, "John Layne" <John------

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On Oct 24, 5:10 pm, "John Layne" <John------

I've done them both in plastic part assemblies, and have had issues to contend with later which gave me problems. I just didn't have the time or patience to know whether there was a solution.
Other posts in this group on External References can be searched for other comments people have made (172 posts). I know caution is recommended. Rereading some of the posts again was a good refresher.
Hence, I eventually break the links after the conceptual sizing is done, so each part file has all its own sketches and has no linked features. I seem to recall issues with multiple configs and then generation of cavities, where things "broke", and this was in SWks 2005 as I recall.
Bo
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Hello Bo,
Ya know, as a Pro/e user, I think it extremely sad that the answer to the problem is to break the links. The whole point of a relation based modeler is totally useless, per SolidWorks, period! SolidWorks Corporation has clearly and consistently shown they have NO CLUE how to manage and provide the proper content and tools for Top Down Design!
.. (I really hate this program!)

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Well, I hope SolidWorks gets better. But I don't have time to flog it.
After spending a week or so on a good size design project, only to find I keep getting problems with External References, I simply find I do NOT have the available hours to keep hammering my head trying to fix things that don't readily work. I revert to simpler files.
I need to be able to get a usable solution now. The user shouldn't have to use elaborate workarounds. The user should not be given tools/ features that are claimed to work, but only work in simple instances.
I'm not slamming SolidWorks, as it is just a tool, and I've learned to keep my files as simple as possible.
I often wonder if an error checking routine in SolidWorks couldn't explain to the user why certain errors ocurr. Again, that is what all that computing horsepower is for, to make our life easier and more productive. Lots of free clock cycles are sitting there waiting for a good debugging utility for users.
Bo
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I find that there is a point in product development where links should be broken. Definitely by the time a part is released for production. However, until that point...
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If they're broken, you can't use them again for another design. What is the reason for breaking vs locking? I've always wondered...
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On Oct 24, 8:10 pm, "John Layne" <John------

I agree in making a part with multiple sketches (and no features) for layout purposes. This part file can be put into any of your assemblies to drive other parts, without referencing out side of the assembly you are in, and all your assemblies are basically linked by this layout file. The other part file you may want to consider putting in each assembly, is one with reference planes, these planes are to be used when designing. In the event that a height or length has to change and this will effect multiple parts, you only have one place to go to make the change. These planes could be made in the layout file, but sometimes it may be cleaner and simpler to keep these two files seperate.
Mark
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I started with #1 and have migrated to #2, as I so often do in other daily situations.
I found that having the layout sketches in the assembly makes them available only in _that_ assembly. With method #2, the skeleton part makes the layout sketches available to be used in any subassembly.
The only drawback (I haven't found others) is that I have to remember to set the skeleton part to be excluded from the BOM. I used to use envelopes for the skeleton parts, but I often need to reference the skeleton part from a higher level assembly. For example, mating a subassembly by one of the layout sketch entities.
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I forgot to add that I don't necessarily limit my skeleton part to sketches and planes. If there is some feature that serves the layout function, it's worth having in the skeleton part. Just set the density as low as possible, or make it a surface feature so it doesn't mess up mass property calculations.
I commontly work to a customer's part model, so that gets inserted into the skeleton part. I make my layout sketches around this model, and only reference the sketches. That way, when they send me a revision of the model, I can instert it, update the layouts, and all of my assemblies are updated to the new model.
I don't get the problems with in-context relations that Bo and Paul metion, but I'm not doing mold work or surface modeling either. I don't have in- context relations to the complex geometry where faces, edges and vertices get lost so easily.
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Interesting -- I've asked this question on comp.cad.solidworks the SolidWorks Forum and SolidMentor --
Getting a lot of different differing points of views and all from people in the SolidWorks community that I trust and respect -- damn there are no straight forward answers.
John Layne www.solidengineering.co.nz
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On Oct 25, 1:11 pm, "John Layne" <John------

If I remember correctly, a fully constrained sketch that is used as an External Reference does not carry the dimensions into the other part, so I think you have sometimes have issues with dimensioning on drawings.
Check it out in your own files.
Bo
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For the most part I tend to use a variety of different techniques.
I generally have some sort of layout sketch, such as a general plant arrangement layout, a conveyor layout, etc. I will put this into a part file so I have more leeway as to hiding, suppressing, moving, etc in the assy, and mate it into the assy with something major at the origin. Depending on what the job is, this may be a column line, or it could be the center of a transfer - a work point - just depends. I may have a car body outline part that has three sketches in it - front, side, top, again mated in whatever fashion is appropriate. Then I usually find that as my design progresses, I may add some sketches in the assy to help define the location of something, or give me some ref dims to watch as I work around something else. These are all the basis of whatever I am designing.
Then I start with something like the carrier that will handle the body. This will go into the assy in such a way as fits the scope of the job. Maybe I want to be able to move it along a path and see how it chords around the curves. I may have a fork transfer that moves the car from an inverted carrier to an overhead carrier, and that transfer is mated with its system planes to the assy, usually to part of the layout sketch. I might have some tooling that travels with the carrier, so it gets mated to the carrier in the assy.
So, as you probably already know, there isn't one right answer, and probably not always even just one that fits the job. Having many tools in the box, and enough experience to know how and when to use each one, generally leads to a better SW experience.
WT
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