Pack and Go a necessity?

[Anonymous]

Hey guys,

So i do sheet metal strictly in inventor, and do shop drawings to be approved by the consumer.

I was talking to my buddy that says he uses pack and go in solidworks and it updates all his drawing files and saves them so it practically does the drawing file for him after he sets up a "template" drawing file, you could say.

So ultimately my question is, is pack and go a good option to use besides just trying to put all the part files into an assembly to send to someone else?

I do a lot of the same items just different dimensions so i was wondering if our pack and go could work the same as the solid works version? That'd save a lot of time on my end and get my shop running faster.

[mcgyvr]

@Anonymous  You misunderstood your friend..

Pack and Go simply gathers all necessary files and can put them into a zip folder to allow you to send native files to others. 

It does not do drawings for you..

Pack and Go: Gathers all related files for a model design (parts, assemblies, drawings, references, design tables, Design Binder content, decals, appearances, and scenes, and SOLIDWORKS Simulation results) into a folder or zip file.

[JDMather]

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@Anonymous wrote:

I was talking to my buddy...

...i was wondering if our pack and go could work the same as the solid works version? 

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I am not aware of any differences between SolidWorks and Inventor in this respect.

Can you ask your buddy to join this discussion (and then provide example SWx dataset)?

[Anonymous]

Im pretty sure hes not working today so i cant get that from him.

and i might've said "do the drawings for you" Wrong.

i was just wondering if i draw the attached file, then draw something similar to it just different dimensions,

is there a way to auto update a new drawing, without messing up the original.

or do i just have to suck it up and just keep doing what I've Been Doing where i just start with a blank page everytime and having to do each dimension and view manually?

[JDMather]

Sketch1 in your part Top.ipt is not fully defined.

This is not best practice in Inventor or in SolidWorks.

I know exactly what your buddy is doing and it would work exactly the same in Inventor, but in first hour of first day of CAD 101 you should have been instructed to choose a logical datum and constrain your sketch to the origin.

All other logical and predictable results follow from that first principle.

Are you interested in learning how to do this correctly?

[Anonymous]

Yes! Im always down to learn new ways and to learn how to use certain features the right way.

[jtylerbc]

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@Anonymous wrote:

i was just wondering if i draw the attached file, then draw something similar to it just different dimensions,

is there a way to auto update a new drawing, without messing up the original.

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The way you describe it here, Pack & Go could be used that way, but it isn't the only way to do it (will come back to that in a bit).  All of this assumes you're not using Vault.  If you are, there are probably methods you could use from Vault that would be preferred to any of these solutions.

Let's say you had a sheet metal part and it's drawing, and wanted to make a similar part with its own drawing.

To separate the new copy from the original, you must do one of two things:

1. Seperate the files into a new Project.
2. Rename the files to distinguish them from the original.

You could use Pack & Go to make an independent copy that you can change separately.  The new drawing and new model would be tied together, with neither referencing the original.  However, the real reason that Pack & Go works for this situation is because Pack & Go creates a new Project File, achieving method #1 above.  Thus, you could achieve the same result without using Pack & Go by simply copy-pasting the files into the Workspace of a different Project File.  Pack & Go's specialty is gathering up the files, so if your file structure is simple enough (ex. one part, one drawing), then that tool isn't really doing anything to help you.

If you want to keep the original and new parts within the same Project, then neither of these options are all that good.  Instead, you would want to use the Design Assistant and its Copy function.  You would run the Design Assistant on the drawing, set it to copy both the drawing and the part, and assign new file names (achieving separation method #2 above).

In short, you are absolutely correct that it can work for this purpose, but Pack & Go isn't really necessary for what you are trying to do, and is taking the long route to get there.

[Anonymous]

oh okay, so i see where your coming from to where it can work out by, in short, copying all my files to another folder (including the drawing and presentation files) so even though they are the same part, they have no relation to eachother anymore?

So i can change the length of the top or height or whatever of the copy without it messing with the original at all.

Also to answer your question, I dont use vault considering when i asked about it earlier on the forums, i was told its not necessary if im the only one accessing my drawings and parts. But i would definitely get vault if that would be the easier/most efficient way to get my desired answer.

[Curtis_Waguespack · Accepted solution]

Hi @Anonymous 

Pack and Go is just gathering up related files and copying them to a new location, and then updating the internal links within so that they are no longer linked to the original files, this allows you to makes changes to the new files without them updating the originals, however its not the best practice to have design files of the same name that differ, and using pack and go in this way is likely to create a giant mess very quickly.

A better approach would be to stop and adopt a proper naming scheme and folder structure.

As an example, we'll imagine that your design reuses most of the components and there are really only a handful that change from design to design...  this example might or might not be the case for you, but it will demonstrate the best practices for you to consider.

So let's say re reorganize your setup as such:

These are the "custom" files named and filed in a folder reflecting their "project" with a prefix of CA50

These are the "library" files that are reused among common designs (again this is just for example, and might not reflect your real world scenario) 

You could then open the assembly file and click the Copy button and select the top level assembly from the browser, this will bring in all of the files into the copy tree, where you can use the "dots" to control what is included, reused, etc.

Here the yellow dots are the reused items, blue are the ones to be copied, gray would be omitted 

here the file names and folders are set, note that we need to select the "Open In New Window" button to copy the top level assembly

This will create the copies of the top level and the components to be copied in the new folder as you specified. Note they will only be in memory until you click Save for the first time and then they will get saved to the new design folder (CA-51 in this example)

So now you would just manually copy over the drawing file in Windows Explorer from the CA-50 folder to the CA-51 folder and rename it from CA50.dwg to CA51.dwg 

Then just open the CA51.dwg file and use the "Replace Model Reference" button to update the drawing links from the 50 to the 51 assembly 

Now you're set up to make design copies in an organized manner without creating a lot of duplicate files and no mess. 

This might take a bit more forethought and planning on the front end and seem like more steps than the pack and go method, but having an organized and well thought out folder and file naming scheme will pay off in a huge way in a very short time... versus using the pack and go method to create different files of the same name, which turns into a mess very quickly.

Note too that there are other methods for copying designs in Inventor to be aware of as well:

https://cadsetterout.com/inventor-tutorials/copy-an-autodesk-inventor-design/

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Wow! Thanks for the steps!

I will Definitely try to get used to this, it seems so helpful.

Also i know how messy it gets when things aren't organized so ive pretty much been doing each job file, each item number, and then all the components so nothings getting mixed up. 

And just making sure, i can still edit and make changes to the copied files just as if i made them from scratch?

[Curtis_Waguespack]

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@Anonymous wrote:

And just making sure, i can still edit and make changes to the copied files just as if i made them from scratch?

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Hi @Anonymous ,

Yep, once the files are copied (as 51 files in the example) they are new independent files and the 50 design doesn't even know they exist.

Another tip that might help you keep track of which files are looking at which files, is to go to the BOM editor in the assembly and click the Column Chooser button and locate the FilePath property in the list, and then drag and drop it into your BOM grid, so that you can see the file path... if you do this in your assembly template, it will be there for all of the new assemblies you create from that template

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[jtylerbc]

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@Anonymous wrote:

oh okay, so i see where your coming from to where it can work out by, in short, copying all my files to another folder (including the drawing and presentation files) so even though they are the same part, they have no relation to eachother anymore?

So i can change the length of the top or height or whatever of the copy without it messing with the original at all.

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Correct, but only if the two folders each have their own Project File.  Having multiple files with the same name in the same Project leads only to bad things.  Also, I gave a very simplistic example, but the methods I listed work for more complex situations with assemblies as well.

Note that it can be confusing having files with the same name even if they're in different projects, so this may not be the ideal way to handle things.  This method is more of a bare minimum to make it work, rather than the best practice.  An organized naming system like what @Curtis_Waguespack describes would be better.

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@Anonymous wrote:

Also to answer your question, I dont use vault considering when i asked about it earlier on the forums, i was told its not necessary if im the only one accessing my drawings and parts. But i would definitely get vault if that would be the easier/most efficient way to get my desired answer.

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I did not mean that you need to get Vault to get what you want.  Just that if you're already using it for other reasons, it could help with this as well.  There are too many other ways of dealing with this situation to be worth introducing Vault just to solve it.

Of course, the advice that @JDMather is giving about your modeling technique needs to take precedence over copying things.  Reusing work by copying files is a smart move, but only will only pay off if you aren't starting out from originals that had problems already.  You'll want to get the model cleaned up according to his suggestions, then start using whatever copying method you choose to go with.  Propagating issues by copying flawed files will cause you problems for years to come, so it's best to get the models right first.

[Anonymous]

Thank you guys so much

This really helps.

Also i understand that if i copy a not finished drawing, ill be fixing mess-ups everytime, that's why im always down to learn how others do it and show me things i dont know before.

I am teaching myself this program whenever im not asking questions here so some of my things might not be the best.

[Anonymous]

Whenever you have the chance, Im eager to learn where i've been messing up haha