Locking out Geometrical Sets from Editing

[Abaddon]

Is there a way to take a geometrical set and lock out the surfaces that are in it from being edited?

For example,

We do almost all of our work in surfaces, and we start with the customer part data, expand it, etc.etc.etc.

I want to be able to Lock out the geometrical Set with the Customer Data, so that its always retained with the part file for verification, but I want to make sure another user doesnt accidentally edit it.

Thanks

 

[solid7]

Are you asking how to protect a surface, so that it may not be deleted, or how to prevent the surface parameters from being edited?

Normally, when creating surfaces, I don't release parametric surfaces in the output models. I keep a parametric model for "reference", and output isolated elements. There's a zero percent chance that your customer will edit a surface in that regard.

I'm not sure about "protecting" the data, but it's a good question, and it's got me wondering (and searching) for myself.


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[jec3300]

I do not think that there is a way to lock a geometric set. On e thing that you can do is to brake the link so that the surface is "dead" this will stop them from easly changing the surface but not replacing the surface.
Hopes this helps

 

[solid7]

On e thing that you can do is to brake the link so that the surface is "dead" this will stop them from easly changing the surface but not replacing the surface.

I'm not sure what you mean by "breaking the link" - I think you mean isolating the surface. But in any case, that's essentially what I was saying, with one major exception. It's a better practice to keep the model parametric, if you need to have parametrics, in the first place, but to "paste special" the data "as result" into a new file, to be used as ONLY a customer package. There's no sense in shooting yourself in the foot, just to keep everyone else honest.

I'm still searching for a means to protect the surfaces.


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[catiajim]

Use Copy/Paste Special/As Result with Link. Then keep your Parametric Surface part in a separate file. You now have the Parametric Surface still linked to the Design, but kept and maintained separately. In the user Part, you will see the surface as an External Reference. The user can use it all day long, but cannot modify it.

It is best, also, if you Publish the Surfaces before performing the Copy/Paste operation.

 

[refross]

Sound as if you are doing Plastic Molds? if so, your problem isn't trying to lock a geometical set. You problem is that you are working directly with the customer data! You need to create a Product with the customer data as a referenced part in the product.
If you are building Plastic Molds, I can discuss it more with you if you like.

 

[flangewiper]

Yes, I agree with the last few posts, I would keep the customer data in it's own part and then publish the elements in this part using Publication from the Tools drop down menu. These will then be created as published elements and duplicated at the bottom of the tree under 'Publication'

You can then copy and paste these elements into your working part with 'Part Special'. If you use the 'as Result' option the element will come in as dead elements with no link but if you use the 'as Result with Link' option a link will be created which is useful if you want interrogate the element and find out where it came from (it will be pointed back to the source part i.e the customer data part. It can also be handy if the customer sends modified data, the link can be used to assist in automatically replacing the old customer data with the new in your working part. The copy / paste operation doesn't necessarily need to performed within a product, but if you don't, and then subsequently open the target part (the one you pasted in to), the link to the source part isn't automatically created. You need to created the link using 'Links' fron the 'Edit' drop down menu, select all the links and then click 'Load'

Hope this makes some sense - it's tricky to explain but is a fundamental and very useful aspect of V5 and probably worth trying with a couple of scrap parts if you haven't seen it before.

 

[Abaddon]

"Sounds as if you are doing Plastic Molds?"

Specifically compression tooling, but same principal being used.




ok guys, this is the point I am at now...

I have a CATPart file.

I have done my expansion, translation, rotation, and have split the data into two Geometric Sets: Cavity and Core.

I have made "Cavity.CATPart" and "Core.CATPart" files within an overall product file for the job. I am aware of the "as result with link" option, but it isnt comming up when I try to link the customer data to my new "working" files. I select the geometric set I want, copy it, and when i select paste special it only gives me the options of "as result" or "as specified in part document".

Does as result with link not work for geometric sets? I have tried doing this with an Ordered Geometric set and nothing changed.

Any and all input is appreciated.
Thanks.

 

[solid7]

It doesn't work on the set itself - but rather individual elements.

You must select a single element, whether that be a solid body, a join, a line, etc... As it is, geometrical sets are just placeholders. You could, of course, select each element. (I've never tried multi-selecting for a paste special)


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