I have a someone that works with me that always inserts part into other parts instead of assemblies. Can anyone explain to me any advantage to this method? What about disadvantages?
Inserting parts in an ASM let's you have most control over all parts involved even if none of the parts need to be dynamically moveable.
Inserting parts in another part has the advantage that it's quick, the disadavantage however is that you lose lots of control and flexibility.
Imagine have a part that is a table and a part that is a chair.
If you put the chair in the table part then you only have 1 part to bring into a higher assembly(let's say ASM "room") with as result that the chair is positioned in reference of the table because you set it up in the part. However, if you come to the conclusion that the chair needs armrests then you'll have to delete the chair part out of the table part. Make the necessary changes on the chair part, and re-insert it into the table part.
If you leave them as seperate parts then you can either bring them both in to ASM "room" or you can make a different ASM, let's call it "combo" and then bring ASM combo into ASM room. No matter which of those two options you use it still means that you have full control over both parts concerning not only the positioning of each other to each other but also concerning using different config's or making changes to either or both of them in a very intuitive manner. You can even make it so that the one influences the other, e.g. longer table means more chairs added by means of an equation.
-part in part can have it's advantages but in general only if you are truly sure that the inserted part won't need to be altered in anyway.
Personally I only use it as a quick&dirty method when time is very precious.
-part in assembly can take longer to set up but in the long run it will save you time and leave you much more freedom to adjust to changes
All depends ofcourse on what one designs/draws, what rules to adhere to, company policy and personal preference or in other words "your mileage may vary".
Their is no advantage and disadvantage, they are different techniques with different purpose.
Multibody parts should not replace the use of assemblies.
A general rule to follow is that one part (multibody or not) should represent one part number in a Bill of Materials. A multibody part consists of multiple solid bodies that are not dynamic. If you need to represent dynamic motion among bodies, use an assembly. Tools such as Move Component, Dynamic Clearance, and Collision Detection are available only with assembly documents.
Not to be disagreeable, but this information is just wrong. If you insert part A (chair) into part B (table), and then modify part A, it will update in part B. You can alter to your hearts content, and part B is updated to match (provided that the referenced part, part A is open). I do this all the time. It is an excellent way to reuse geometry in multiple part and have them all linked back to the master part. The only caveat that I'd add is to insert the part as soon as you can in the feature tree, as the 'Move/Copy' feature imbedded within the 'Insert Part' can get messed up if a feature before the insert is changed/deleted.
I did notice in my experiment that updates to the inserted part were reflected in the part that it was inserted into.
Thanks for the information about the feature tree. That could cause some major issues.
Your welcome. BTW, usually, if the Move/Copy does get messed up, you can just add another one outside the scope of the 'Insert', and re-orient the part to where it should be.
Also, there is a box that can be checked to break the link between the part if needed or desired. It's unchecked by default. However, it only seems to be available for the first part inserted into a part. All subsequent parts that are inserted don't have it. SW might be using the break external references function (all or nothing proposition) to do this, which would sort of make sense.
Ok, just for giggles, I tried that check box, and indeed, it does break ALL external references, not just the part being inserted. Without warning!! And they cannot be undone or fixed. Seems like really bad practice by the SW programmers. I don't think that I'll ever touch that again.
I stand corrected. If you insert part A into B and then alter A you'll see that it will have changed in B.
The reason I didn't think about that is because if and when I use part in part then the part I insert always has configurations.
My experience is that if part A has multiple configurations then the only configuration that you'll see after inserting is the one that was last saved when inserting it into B. Which means that if you have a chair with 2 config's, one with armrests and one without armrests and you have last saved that part with the config being active without the armrests then I know of only two ways to get the armrests in the inserted part.
1/ add armrests to the config without armrests, which kind of defeats the purpose of having the config in the first place
2/ re-save the part so that the armrests are active and then re-insert the part.
If you know of an easier way then I would gladly hear about it. Especially if you know a way to select a different configuration of an inserted part.
Have a nice one
Peter, just right click the part and list external references. From there you can change the configuration of the inserted part.
Ah okay, thank you kindly.
I never thought about checking external references for a part that is already available. Not exactly the most intuitive path but it gets the job done.
As Chris noted, you can change the configs. Also, an advantage to inserting a part in a part, is that you get to select what type of geometry that you want to insert. So, if the chair model contains unabsorbed sketches, reference planes, construction surfaces, and a solid body, you can insert only the finished solid body, and not all the other unneeded stuff. Or any combination of types.
I personally try to avoid Part in Part due to it creating external references that have to be read every time. I believe I read somewhere on these forums before that it takes longer to resolve and load than just using an Assembly. Correct me if I am wrong. I've never actually tested this myself.
If the external reference hasn't changed, then it doesn't need to be loaded. There is an option under Tools, Options, System Options, External References, to control when to load referenced documents. I usually set this to 'Prompt', so that I can load them when I know that they have changed, and leave them unloaded when I know that they haven't. When left unloaded, there seems to be no time spent resolving them, so they are faster than an assembly.
I use them typically to insert 'tool' geometry into a part. That is, geometry that will be used to create another part, not to insert a component into a part. For many of the parts that I work on, this 'tool' geometry is huge and takes a long time to rebuild. Once it is inserted into a part, and the part is reopened without loading the referenced part, the part loads and saves far faster (sometimes it can save as much as 10 minutes, per save!). Also, it results in a far cleaner and easier to understand feature tree.
A right click on the inserted part will show "Edit in context" which opens the part and lets you edit all you want.
As Peter and Ahmed have said, there are appropriate times to use both. It's difficult to critique your coworkers workflow without knowing more about what type of modeling you do, but pretty much the only time I insert a Part into a Part is when hardware, such as a hex nut, will be welded onto structural steel. Everything else is an Assembly. They're just easier to work with and easier to edit.
Thanks to all that replied. The feedback information is very beneficial.
Since I have always used assemblies before I did some experiments to see if I could find any differences. The two main issues that I found were: 1 BOM tables don't show these parts and 2. EPDM doesn't show the inserted parts in the "contains" tab. Neither of which are show stoppers but probably not best practices.
I will discuss with the originator to see if they can explain why it was done this way and what benefits it has over assemblies.
Again, Thanks to all.
As usual, when I make a definitive statement it comes back to bite me. Not an hour after I posted above about only inserting a Part into a Part if it was welded together I needed to create a wedge type concrete anchor. I could have done it as an assembly, but made it a single part instead since it's sold with the washer and nut. This one isn't perfect, but it's close enough; and I rarely model threads.
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