Creating parts library question

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Jenny
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Creating parts library question

Post by Jenny » Wed Nov 21, 2007 7:06 pm

I'm currently trying to create some components. I've gotten as far as making up a component and creating an excel sheet for additional sizes.

Currently I'm working on a travel strap. We have a number of standard sizes for these depending on the size of mold.

Couple of questions, firstly I'd added my screws to this part, but I"m not sure I've done it the proper way. I first created a *dummy block* for my tools, then added the screws through Assembly/screw. How do I now add this to my excel sheet? I try to bring up the driving elements for the screw and it does not give me anything dimension wise that I would be able to define as a driver.

I need to be able to change the size of the screw as my travel strap gets bigger. Any suggestions?

My second question is can you add and omit items on a component when making a library part. Example: slide gibs. We have standard sizes that we use, the smaller length gibs only have two screws where as the larger lenght gibe have three. Any ideas??

Thanks!

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Larry M.
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Post by Larry M. » Wed Nov 21, 2007 7:21 pm

As far as I know Jenny you can not have it change screw size by the exel spread sheet. The only way Ive been able to do it is by making my own bolt and driving all the parameters of it. Or adding the bolts after I insert the strap.

Jenny
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Post by Jenny » Tue Nov 27, 2007 7:32 pm

Thanks Larry,

What about omitting certain features in a library part using excel?? I tried just leaving dimentions blank and it gives me errors. Any ideas?

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Larry M.
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Post by Larry M. » Wed Nov 28, 2007 7:07 pm

Just get rid of the column for that parameter. Or just put in the same number for all of them.

Jenny
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Post by Jenny » Thu Nov 29, 2007 3:51 pm

Sorry I'm confused, if I delete the column, will that completly remove said feature from all my parts listed in that excel format?

For instance, we have standard knock out extensions. They come in numerous lengths depending on the size clamp plate you're using. They also come in 1/2" tap, 5/8" tap and no tap.... How do I remove the tap completely from one part in my excel sheet and not the others??

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Larry M.
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Post by Larry M. » Thu Nov 29, 2007 4:04 pm

As far as I know with Library parts, And I've done a lot of them, You can not add and remove features by parameter, like a tapped hole.

You would have to have 3 different library components in that situation.

I haven't been able to figure out how to switch tap sizes in a component with an exel sheet yet.

My best guess would be put in a hole only (tap size) drive that with a parameter, and then tap it. TS should automatically pick the tap size. Then you might be able to have it switch tap sizes.

But you can not have it turn features on and off, If the master library component has a tapped hole, all of the different components you create with it will have a tapped hole, you just can change the size and depth with parameters.

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Post by Aaron A » Wed May 06, 2009 2:12 pm

I know you have probably solved this problem but I would just like to post for future readers:
You CAN add or remove features by parameters - go to shape/manage/deactivate operations and click on "one operation". now click on the operation you would like to control. next type in a variable that when true the operation will deactivate. If you do this with a parameter like Ø==2 then when Ø is equal to two then the feature is deactivated.
To change tap sizes with an excel sheet use the modify element tool (the wrench) and click on the tap size (if you can see the driving elements). in the list that appears there will be an option "parameter". click on it and in the nominal value field type in the controlling parameter (Ø). whatever value Ø is will control the diameter of the tapped hole, though be careful only diameters that are equal to the ones in the library will work (example .312 for 5/16).
Enjoy

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