Re-Usable geometry

[multicaduser]

This may take a little explaining so apologies first. Real world projects are best for learning so I've been using AD Expert to design dust collection adapters for my wood shop stationary equipment. Now I want to move onto the portable and hand held tools and want to develop a bayonet adapter for a single connection point for multiple tools. I'm very comfortable with configurations and am thinking of using them for the adapting side, having the bayonet geometry fir the base feature with the adaptive side for each tool defined by each configuration.

The up side is that there is one place to adjust when making changes for fit and function on the bayonet side along with having a single file to add new adaptive configurations. One down side is one file contains everything and if it gets broken all can be lost. The soon to be released pdm system may help with those fears and I'm very diligent about versioning when making large changes, but all the eggs in one basket is not just a warning.

Does this seem like a reasonable path and is there another option which might serve as well? I've learned a lot from long time users on this forum and hope to get enough experience to be more than just a lurker.

Thanks in advance for any replies.

 

[NateLiquidGravity]

Configurations could be used but the part file will only have one file name and one icon. I would make the base geometry in a separate part that is inserted into your adapter parts as a Boolean feature. Then make a new part for each adapter. That way the base geometry can be edited separately and any changes in an adapter part won't affect the base geometry or any other adapter part.

 

[multicaduser]

Hey Nate, thanks for the reply. Boolean's are something I thought of shortly after hitting post. I've played with them but haven't had a real world use for them yet, but it sounds like this will be the perfect chance as I have time this weekend. Are there any caveats with using them as far as updates, etc.? Thanks again.

 

[Ex Machina]

Nate approach is probably your best bet for what you're trying to achieve.

 

[NateLiquidGravity]

Using boolean features - all changes to the boolean tool parts will propagate through when the file is opened. And like any other things those changes can break things depending on where in the part history you put it and how you build to it. For example if you remove a face in the boolean tool part then any fillet that was using that face can break.

 

[multicaduser]

Thanks @NateLiquidGravity , a combination of configurations and boolean unite features is going to help standardize and control designs like I didn't think possible. Every time I learn something new in AD the more impressive the software gets and the quick responses on this forum saved a lot of development time. Not 100% sure about the update when changes are made to the origin of the boolean features but I read on the forum something about commit and hitting F5, neither of which worked until the target part was added to the assembly. Will have to read the docs more.

Thanks again.

 

[DavidJ]

If you have a part containing a boolean open, then separately open the boolean source, you now have 2 separate instances open in memory from the one file on disk. Changes in one memory instance won't show in the other, and what's more if you save files in the wrong order you can lose changes too.

Generally best not to have both open at the same time...

 

[multicaduser]

@DavidJ , are you saying then, that having both files in an assembly is bad?

 

[DavidJ]

I am saying that if you have more than one instance of the same file open, there is scope for confusion and even data loss if editing.

Examples include
* Editing a separate instance of a part file, when the assembly it is contained in is also open ( to avoid problems use 'edit here' or 'edit in separate window' from the assembly then you are working with a single instance of the file).

 

[multicaduser]

Thank you for clarifying, I'm very impressed with both the software and the forum. Sometimes it seems people are not as appreciative as they should be.

 

[HaroldL]

Be aware that there is no way to edit the Boolean tool in the the Boolean feature, there is no RMC Edit option.



So, if the tool needs to be modifed you should close the part file containing the Boolean feature, edit the Tool part, then reopen the part file with the Boolean feature and it will have the updates applied to the Boolean tool part.

It would go a long way of making Booleans a more useful if you could edit the tool parts similar to the Edit Here or Edit in a new Window option that assemblies have. And I'm not sure what kind of programming machinations need to take place to implement that feature.

 

[multicaduser]

Had a chance to play with boolean add some more, and this workflow seems to be best for what I'm trying to accomplish.

1. Created an assembly with both sides of the bayonet in a base configuration.
2. Opened the file for the tool side connection and did a boolean add of the require bayonet side to complete the design.
3. Added a configuration to the assembly for the tool side connection and added the model to the assembly. Location is not important for the intent.
4. Repeated steps 2 and 3 for another tool side connection.

After this was done an obvious un-needed change was added to the boolean add model in the context of the assembly, just for testing purposes. In the world of one ring to rule them all, this procedure updated every model with the boolean add in the assembly to include the modification at the same time, which is the intent in this case.

With all the help from forum members this is how I figured it would work, and it is very impressive.