How to add a fastener

[ptc-4279698]

I just started learning creo/elements and I'm sorry if this is a basic question. How do I add a fastener to an assembly? The help pages says insert>connection>fastener. But I don't have a connection choice under the insert menu. Thanks.

[AdamHaas · Accepted solution]

David,

In short, you create an assembly and then insert components into the assembly. Components are placed using constraints such as Insert, Mate and Align. If you select the cylindrical surface of a hole and then of the fastener, an Insert constraint will automatically be created. You would then add a second constraint by selecting the bottom of the fastener head and the surface it will mate against. You could use the Repeat function to easily place multiple fasteners.

For more in-depth instruction, I would suggest you go to www.ptc.com/go/first and in the Training and Resources tab, you will find FIRST specific curriculum as well as links to our basic Academic Program training materials.

Hope this helps.

Adam

[ptc-4279698]

Sorry, I should have been clearer with my question. The Help Center describes a Fastener Definition dialog box that appears to give the user access to a built-in library of fasteners. I’m wondering how I can get to the Fastener Definition dialog box. The suggested menu sequence (Insert > Connection > Fastener) doesn’t appear when I’m assembling parts.

I can make my own fasteners or import them if I need to but it would save me time if I could access an existing library. I guess my other question is why the Help Center doesn't match the product?

[ptc-4279698]

I found an on-line library of fasteners that can be downloaded for free. http://www.3dmodelspace.com/prolibrary.html I don't think you can access it directly from within creo/elements but I started accumulating a downloaded library of fasteners I commonly use.

[AdamHaas]

David,

Now that you are accumulating your own library of fasteners, there are a couple things you can do with them.

1. You could put them in a common folder and then define that folder as your "library" using the config.pro option “pro_library_dir”. By adding this, when you go to assemble a component, you can click Pro/Library from the Common Folders area (left side) of the Open dialog box.
2. If you are putting your standard components in a library folder, you will need to also add a search path so that if you open an assembly, Creo will be able to find the components. This can be done with the config.pro option “search_path”.

An example of the config.pro options I would use to accomplish 1 and 2 above is shown below:

pro_library_dir C:\Users\student\standard_parts

search_path C:\Users\student\standard_parts

[MikkoHinkkanen]

Hi!

The suggested menu sequence (Insert > Connection > Fastener) doesn’t appear when I’m assembling parts

This help refers to Creo Simulate, not Creo Parametric.

To have nice fastener experience, I suggest that you try: IFX.

[Cuong_Nguyen1]

You have to enable this function in configuration editor, you can follow following step:

File --> Option--> Configuration Editor--> Find--> intelligent_fastener_enabled-->yes. and then save config.pro.

Restart your creo.

It will work.

Hope achive good result

[huggre]

David

If you use Creo Parametric 3.0 you will find the IFX menu under Tools->Intelligent Fastner

[OliverGräbner]

Hi David,

could you solve the problem in the meantime?

Maybe you find some helpful discussions or videos about fasteners on Intelligent Fastener Extension - IFX‌.

Thanks,

Oli

[rjohnson-4]

The Intelligent Fasteners are a awesome and very easy to use.  Just select toe Tools tab and click on "Screw".  You then have a couple of steps in sequence...

1. Select the hole where you want to put the fastener.
2. Select the surface where you want the head of the fastener to be constrained against
3. Select the surface where you want the nut to be constrained, or if not using a nut, where threads would normally start
4. Hit ok

You'll then see a dialog where you can select the type of screw (metric, ansi, etc).  Then select the length, width, and nut (if desired).  You can also expand the dialog to fiddle with hole parameters (like tight or loose tolerances).  Hit OK and you'll watch Creo drill the hole, put in a screw, and put a nut on it.  Rather cool!

IMPORTANT: Here's where this can go wrong.  When you need to modify or delete the fastener, don't do it from the model tree.  All those holes, nuts, and screws are connected together, and the connections can be lost if you do.  Instead simply select Delete, Redefine, or Reassemble from the Tools->>Intelligent Fastener portion of the ribbon (where you found the screw).  You'll see the same dialogs from before and can change hole, screw, or length easily.

Good luck!

Rande Johnson

Coach/Mentor FRC 4931, FTC 8620/9998