part vs. assembly 2

[koyote5]

when creating a top down assembly I am often confused as to which plane to sketch on. I could choose a plane from the assembly or the part. Normally they coincude but sometimes they dont. Will one cause a problem. If i draw a part feature on an assembly plane can the part exist outside the assembly. Will it cause a problem? What about if I change something in the assembly and then that causes the pieces to not line up properly? Also is it possible to create the part based on its location in juxtaposition to another part and them move it elsewhere and use mates to position it. Will the features referenced elsewhere in the assembly have a problem updating? Any input is appreciated.

 

[PlasticFantastic]

I try to stay as far away from sketching on an assemply plane as I can. The only exception is to create a skeleton for the assembly ie- a simplified sketch that can help create the mated top down assembly easier (it is easier to mate to 2D sketch entities than to 3D geometry) Although it is very easy to sketch on an Assembly level datum plane, it would be more advisable to pick the part level sketch planes from the history tree as far as possible. The more external references the longer the rebuild times-especially when you recycle a part from one assembly to build a revised part in another newer assembly.

 

[Theophilus]

Plus, it's a good practice to close off your references outside each part when you reach a "final" phase of a part's design--such as production release. This allows you to use the part in the context of other assemblies without all the entanglements of in-context references, and also allows your part to be independent such that you don't need your assembly to have your part. (Ever lost a file to corruption? That would be terrible if the corrupted file was an assembly file from which all your parts were generated.)

If you design in such a way as to gain this independence with your models, you'll have a more robust and independent database of parts.

In the case you mentioned, I normally insert a new part into the assembly and build from there. When I'm finished with referrals to other parts within the assembly, I eliminate them and constrain them within the part's own sketches/features.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[koyote5]

what if you have a piston, for example, which has referenced dimensions to a an engine in an assembly but you also want to use the same part in a diffenrt engine in another assembly. can you set up to use the same part or would they have to be two different part files?

 

[Theophilus]

You can use the same part. However, you will not be able to edit the part in the context of the new assembly unless you delete the in-context references to the old assembly.

Also, note that if you do make edits in the new assembly, the part will update in the old assembly (if the parts are in the same directory).

This brings up document control issues. If the same part is truly the same part (no differences), feel free to use it in several assemblies. If you make any changes, you should change the file name (Save As. ..) so things don't get confused. When you open an assembly, the parts are called into the assembly by file name.

Between major revisions, I normally will open my "master" assembly (that holds all parts and sub-assemblies) for the project, create a new directory (such as 050103 for today's date, within a project directory such as Piston Engine 01), and hit File, Find References, Copy to copy all parts referenced in my "master" assembly into the new directory. I then close the assembly and open the assembly in the new directory to make any changes for the new revision.

This practice is very basic and leaves a good document control trail. It won't work in many scenarios, however, such as multiple people accessing the same parts on a server. In that case, you should consider PLM software or some other document control practices. It's also critical to have a regular back-up process so files cannot be lost in case of a hard drive failure, fire, etc.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[CorBlimeyLimey]

Check out

http://www.solidprofessor.com/flash/Tips/external_refs.html

for SW2005 method of using In-context method, without keeping external links.



Eng-Tips:-
Intelligent Work Forums For Engineering Professionals

 

[TheTick]

Be forewarned that the above-linked page has sound.

 

[CorBlimeyLimey]

Had your speakers up too loud?



Eng-Tips:-
Intelligent Work Forums For Engineering Professionals

 

[koyote5]

heres the real brain itch:
this piston has to be able to move. therefore, is it better to create in context and keep it locked in place (using converted goemetry "on edge" for example) or to create each part separately and then use mates?
Idealy i would like to have all parts in context for a true top down design yet still be able to move them as if they mated. Is there a solution that would allow for both? What if its driven off of a spreadsheet? they have to move but i want all the parts to update automatically by either editing a layout sketch in the assembly or changing values in the chart.

 

[koyote5]

I would like to thank everybody for contributing in my moment of utter confusion. It has been very helpful.

 

[SBaugh]

faq559-871

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
faq559-716 - SW Fora Users

 

[koyote5]

heres what im trying to figure out. if i were to create a part and then import it into an assembly i could then move it around until i had mated it with another part. this can still allow for degrees of movement which in turn lets me reposition the part.
Designing in context locks the part in place. although i can unlock the part and move it around, doing so will create errors in the sketch since part geometry, features, planes, etc. have refernces to the assembly.
Is there a way to have a part's dimensions driven from an assembly sketch yet let the part move as if it's independant?
Can this be done in conjunction with a spreadsheet and will it help or just complicate everything. It would be nice to be able to make several variations of the assembly just by changing some values but it is important that that the parts do not remain static.
Is there SW feature that i am not aware of or am I just going about this the wrong way.

 

[Theophilus]

Yes, you can do what you want--keeping dependent relations to an assembly within a part while allowing movement in an assembly--just not the same assembly as the relations exist.

So, you can create a part in the context of one assembly, then move the parts into another assembly for movement. However, in doing so, you cannot edit the part in the context of the new, movable assembly because that creates logical problems. Each part can have dependent relations in one assembly only. I don't recommend doing this sort of thing, since the possibilities of error compound through the complications it presents (not best practice).

Is it possible to eliminate the dependent relations and keep the relevant parts within their native assembly or will you continually need to roll updates through several parts with their dependent relationships?

These are part of the growing pains in learning "best practices" along the way. Eventually, you'll come to a good set of planned actions before starting assemblies and even parts that will make this roll along much more smoothly--just takes a lot of practice and experience with understanding (difficult to convey in a "teaching" way or tutorial).


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[Theophilus]

You can also use configurations to assign mates within an assembly that are supressed in one config and unsupressed in another config. This will allow one config to show parts in one position and other configs to show other positions, depending on how many you need.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.