Solid Edge How-To: Create Inter-Part Relationships in ST6

Solid Edge How-To: Create Inter-Part Relationships in ST6

In this blog entry, I will answer a question from the last month’s Solid Edge Short covering Assemblies in ST6 (View the webinar replay here). During the webinar, I briefly covered how Inter-Part Relationships are created in Solid Edge ST6 and how a part’s geometry can “drive” another part’s geometry – specifically, how the “rail_side” was driving cylinder placement in the “side plate” part. (Image 1) The question submitted was: “Can this method also drive the size of the cylinders in the “side plate”, and would this method work on if the cylinders were created with the “Hole” command and were threaded?” (Image 2). It is best if I break this question down into two parts. I will begin with the same assembly as before.

Image 1
Image 2

Driving the Size of the Cylinders

1.  Create the necessary assembly relationships between the “rail_side” and the “side plate” part, run the “Create Inter-Part Relationships” command and review the dialog box.

a.  Click on the “Create Inter-Part Relationships” button

b.  Review the dialog box, and note the “Equal Radius” box is checked at the top and the command has recognized the “Equal Radius” in the list.

c.  Click “Save”. Notice in pathfinder, the icon next to the part being driven should change and show two chain links.

2.  Next, “Edit In Place” the driving part in chase the “rail_side” part and create some Face Relate Relationships between the cylinders. This will allow for all cylinder sizes to change at once.

a.  With “Edit In Place” active, rotate the “rail_side” part around to see the cylinders. Then in the Home Tab, locate the Face Relate section and chose “Equal Radius”. (Note: Have the persist lock active)

b.  Following the directions in the command prompt, have all cylinders equal to the one in top left of the part. (Note: When using face relate commands, the sequence is: select seed face > accept (right mouse click) select target face > accept > accept) 

Make all cylinders equal to this one.

c.  The relationships now appear in the pathfinder.

3.  Go ahead and change the size of the hole cut out (top left corner) and the rest will follow suite. Then “Close and Return” to the assembly and see that the cylinder in the “side plate” will automatically change to the new size.

a.  Changed the hole size from .219” to .3”. As soon as the change is accepted the other cylinder changed as well.

b.  Click on “Close and Return”

c.  Notice the hole cut out change made on the “slide plate”

Threaded Cylinders created with the “Hole” command

When using the Hole command to place cylinders not only are you cutting away material you are creating intelligent procedural features. Therefore, when looking at threaded cylinders, there can be quite of bit extra information added to the cylinder.

The “Create Inter-Part Relationships” only recognizes the part geometry in each part to drive one another. It will not take the extra information added by the Hole command and use it to drive another hole in a separate part in an assembly. There is a way to can obtain the same relationship by using a different assembly command.

1. Inside the assembly environment and under the “Features” tab there is a Hole command used to create a threaded hole.

2. A dialog box will display some different “Assembly Feature Options”. The threaded hole will be an “Assembly-Driven Part feature” and will be driven on the assembly level, but the threaded hole will be placed in each individual part.

a. Select “Assembly-Driven Part feature” and click OK.

 

b.  Set the Hole options.

 

c. Place the Threaded Holes on the parts. In this example, I am placing a ¼ inch threaded hole that will go through two blocks.

d.  Next accept the “cut direction”.

e.  Finish out the command. The threaded holes are now placed in both blocks. The pathfinder has a gold chain link indicating that they are both linked and a new entry “Assembly-Driven Part Feature”. Expanding this item will show the entry for the new threaded holes.

3. When the threaded hole size (or any attribute) is changed, the link that was created will make the change in both parts.

I hope these tips will help further your design experience!

Sam Estrada
Application Engineer
Swoosh Technologies

Post by Sam Estrada

Leave a Reply

Your email address will not be published. Required fields are marked *