Questions on standard assembly screw library in Creo 3.0

[Blackhawk]

Hello - I am using Creo 3.0 with Windchill 11.0.  I am looking to start using the included lite version of the Intelligent Fastener Extension.  I had a few questions:

1) How does Windchill handle the standard hardware library?  For example, if I create a screw using the library, what happens when I check it in to Windchill?  How does it work if another user creates the same screw and also tries to check it in?

2) Does anyone know why the DIN912 socket head cap screw option does not contain anything smaller than a M4 size?

3) I notice that the DIN912 option only creates one object in my workspace, but the ANSI-Metric will create a huge list of parts in my workspace even though I only used one screw in my assembly.  Why does the ANSI-Metric screws create family tables in the workspace, but DIN912 does not?

Thanks!

[BenLoosli]

Not answering your questions but raising more issues with IFX.

Using the light version, you cannot modify them to be your part numbers and they come as some generic name and description. In order to modify the tables, you need the full version.

I would hope that ALL of the hardware is in family tables. We used Cadenas for a while, what a disaster!!! Every part was individual and had 3X as many dimensions as needed. A real pain to clean up.

Does DIN912 cover smaller than M4 screws?

As for Windchill. the first user to create a part and check it in wins. Everyone else will have to use that screw from Windchill and not create a new one. Windchill will NOT allow a second file of the same name to be checked in.

[Blackhawk]

DIN912 covers down to a M1.6 size.

I was hoping that there might be some intelligence within Windchill that could recognize the screws created in session and not have to be checked out from Windchill every time.

Not all of the hardware comes into the workspace as a family table.

[TomU]

We don't currently use these but there is a way to manually upload all of them to Windchill.  Take a look at this knowledge base article:  https://www.ptc.com/en/support/article?n=CS183030

[OliverGräbner]

Hi,

here are some answers:

1) The goal should be to have all fasteners in Windchill. Then all user can use these fasteners. It does not make sense to create the fastener for each user (even if this is possible if you do not check it in). It is also possible to add your legacy fastener data to IFX (require the full version).

2) IFX only has sizes from M4 up to M36 at the moment. Of course you can add other sizes if needed. But this also require the full version. If you want you can add a enhancement request to PTC to add other size.

3) There are two kinds of library parts in IFX. One use a single part for each new fastener copied from a template part. The other kind use a family table with all instance for each size. In IFX you find the files with family table in the subfolder <ifx>\parts\prolibrary. In these folder some fasteners from the ProLibrary  are added. 

In addition there are some pem nuts in <ifx>\parts\ifx_fastener_archive.

This is the reason why sometimes a family table is loaded and sometimes only one part. 

We want to give the user the flexibility to work like he prefer.

NOTE: In the new Creo Design packages the full version of IFX is already included without additional payment.

Regards,
Oli

[Blackhawk]

Thanks for all the replies.  Here is how I would like for the Lite version to work.  Is this possible?

I load the Lite version IFX library into Windchill.  Any user then uses the screw creator within Creo 3.0 in their assembly to add screws to their model.  The screws are then added to the workspace automatically.   I would also like to add two parameters to the fasteners for an internal part number and description.  This would be the same parameters for all users. 

I prefer not having a family table for the fasteners as this adds a huge number of items into your workspace.

[OliverGräbner]

Hi, 

adding all fasteners is possible. But you should review the screw/dowel pin catalogs first. 

Remove all content you do not need - especially the prolibrary files, because they use family table parts. (red marked in image)

 

Adding parameters is not supported in the free version. This requires the full version.

But you can reuse the NAMING and DESIGNATION parameters. These are free parameter.

Regards,
Oli

[Blackhawk]

Oli, thanks for the reply.  What is the step by step process for adding the fasteners to Windchill?  

Thanks

[OliverGräbner]

Hi,

in the IFX - Group you find an "Instance Creator".

Use this creator to create all your fastener parts to a selected folder.

Then simply use the normal process to upload the files to Windchill.

But first of all you should be clear if you want to use single part fasteners or family table fasteners.

Regards,
Oli

[OliverGräbner]

Hi,

I also found a movie 

https://learningconnector.ptc.com/content/tut-4154/loading-ptc-creo-intelligent-fastener-library-into-windchill

Regards,
Oli

[Blackhawk]

Oli,

The movie was very helpful, thank you.  I tried the instance creator and selected a folder on my desktop for the export location.  After the export completed, the screws did appear in my workspace.  The folder on my desktop was empty, however.  Is the export folder just used as a temporary location as the workspace gets populated with the parts?

Also, I opened one of the screws inside of Creo.  I am able to add parameters to the part.  For example, I added a "part_no" parameter and Creo accepted the edit.  I closed the file, emptied my memory, then re-opened the file.  The "part_no" parameter was there.  It seems that I can add parameters or am I missing something?

Thanks

[OliverGräbner]

Hi,

the export folder is needed if you work without Windchill. Then you can create all your file in an archive folder and add a search_path for this location. If working with windchill the files are stored in Workspace.

Of course you can modify the part after creation. The check for a valid fastener for the free version will take place while assemble this fastener. Then your "part_no" parameter will not be accepted.

Regards,
Oli

[OliverGräbner]

Hi,

just a short follow up. Could we answer your question?

If so, please mark this post as solved.

Thanks
Oli

[BenLoosli]

You cannot modify the files in the Lite version to add your own numbers. You must buy the full version to do modifications.

Family tables only add 1 extra part to your workspace, the generic, if done properly! I have family tables of hardware items with over 700 instances and pulling 1 instance into an assembly and then saving the assembly only adds the generic and the instance used to a workspace. There are preference settings that need set for it to work properly.

[Blackhawk]

Ben - Could you give me more info on how to do this?  What preference settings need to be changed?

Thanks

[BenLoosli]

It will take me a while to look through them, but I will try to find them.

One thing we do is have the family tables in a library in Windchill and set the preference that library objects are read-only when pulled into a workspace. This reduces the ability of the end user changing a library part. Only 2 of us here have librarian rights to modify library files. You can set Creo with a config.pro setting to not regenerate read-only objects, too. This helps for both library and released parts.

[BenLoosli]

Open the Quick Links button on the tab right of your Windchill browser.

Then My Settings and Preferences.

Expand the Workspace settings, Add to Workspace and Check out and Add to Workspace Collector.

These should be set to the default, but check these

Include related family table objects and set to none

Include related Generics and set to none