Backing Up Parts

[CADSD]

Lets see if I have completely missed something here or not. I have parts that are for machine ops. I want to have a version for my assemblies (no tool ops) and one that I tool path (mem hog). So I have a copy of the the part ready to start toolpthing but it does not have refrences to the original hence will not update if I make changes to the original thats in my assembly.
Any ideas? Thanks

Jake

 

[JMirisola]

Configurations. Or, depending on the complexity of the machine ops, you could bring the base part into an assembly (by itself) and do the cutting in there.

Jeff Mirisola, CSWP
Director of Engineering
M9 Defense
My Blog

 

[CADSD]

Thats what I prefer is to have the original part in the assembly and the machine setup in its own file, a lot of these parts have ops on all sides. I was also just thinking it would be a nice way to back up parts if I could create essentially a "parent" part that has its changes updated to a copy of the part that I save on the network.

 

[ctopher]

I agree with Jeff, use configurations.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[CADSD]

How would that work in this instance?

 

[ctopher]

Have you used configurations?
Try YouTube.

http://www.youtube.com/results?sear...=70l4696l0l4930l16l16l0l8l8l0l513l513l5-1l1l0

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[CorBlimeyLimey]

Create the part as it would be in real life.

If the part is actually machined while in an assy, then (as jeff suggested) insert the part into an assy and create the machining operations there.

If the machining is performed at the part level, the create the machine ops at the part level using one of two methods;
1) If starting from raw material .... Select the Suppress features option in the Configuration Properties > Advanced Options section, create the first machine op feature, create new config and add next machine op, create new config and add next machine op, etc.
2) If starting from a purchased part or modifying a standard part ... Start new part, insert base part add configs and machine ops as per 1).

 

[CADSD]

I think we are missing the point, I want to save two copies of the same part and have one be the master on which I work, and have the second on another media device as a back up which uses the first as a reference. But it does not look like I can set a part to have a part reference. How do you guys then back up parts? You don't just have one copy right?

 

[ctopher]

I use CAMWorks and PDMWorks. The CAM data stays with the part file, the part file is checked into the vault (server).
Backed up weekly and all versions/history are saved.
This also saves drive space.

If you don't have either, I suggest make a backup folder on a server and backup nightly.
If you want separate backup copies of each version you make, I then suggest installing several terabyte drives.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[CorBlimeyLimey]

Having a 'backup' copy which is automatically (or manually) updated from the working master would defeat the purpose of having a backup.
If the working master becomes corrupt, that corruption could be copied into the backup copy.

At days-end, I copy anything I worked on during the day to a flash drive, and if necessary copy to my home computer for further work.
Every weekend I backup all the company computers active directories to external drives.

 

[kellnerp]

CADSD

Well, you can create a new part and insert the driving part using insert part. The second part will be a dumb part. You can do additional things to it, but any changes to the original will not back propagate.

If you have Utilities you can search and delete small fillets and the like and use delete face to remove them making that part more assembly friendly. Of course that will blow away any kind of top down design.


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[mjcole]

Using the Insert Part option as Kellnerp suggested you will get The Part body inserted to the feature tree of the model as an External Reference -> and you will be able to access the original file by right clicking and choosing Edit Part In Context

Insert Derived Part
Under Transfer options, you get to decide what information to bring in from the parent part.
Custom properties, Solid bodies, Surface bodies,
Axes, Coordinate systems, Planes, Cosmetic threads,
Sketches - Absorbed (used) & Unobsorbed(unused),
and Model dimensions/Hole wizard data. from the inserted part.

The Features of original part won't show in the derived part but the data will update when originaaal is changed. Any features made in the derived part cannot be seen on the original.

Using Configurations you can set your Solid non machined features to exist. and add the option to supress any new features so you don't have to supress them in the As CAST model configuration.

I'm sure you can test each method and see which has the best benefits for your process.

Happy New Year Everybody!


Michael


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