NX7.5 Slot.

[nkward]

I'm having trouble putting a slot in a sheet metal part.
First off, the reason I want to use the slot feature is so I can dimension to the center of the slot(aka, add a centerline to the center of the slot) and not the ends.
If there's an easier solution to this then stop reading and let me know what that is.
Also, if by using the slot feature, I still won't be able to dimension to the center, than this is pointless.

I literally don't understand what the slot command wants.
When doing the slot feature, I pick rectangular, ok,
asks for planar placement face. I select the face where I want the slot.
asks for horizontal reference, pick a face 90deg from planar placement.
asks for thru face and even when I select something parallel to the horizontal face. I get an error message asking to pick something parallel to the horizontal face.
makes no sense.

 

[nkward]

Figured it out with offset centerlines........
disregard the thread.

 

[nkward]

Unless there's a projected view at an angle.
The offset centerline only goes horizontal or vertical, without a reference to what is horizontal or vertical.....

 

[nkward]

Ok, added a circle at the center of the slot in the slot sketch. Made sketch layer visible in view to create centermark. Then made sketch layer invisible in view.

Slots shouldn't be this hard. It should be a function of the hole command with a reference direction and length.

 

[JohnRBaker]

The 'Slot' function in NX is actually intended for machining a 'slot' in something like a plate of steel. What NX is actually missing is a 'Slotted Hole'.

That being said, go to the 'Reuse Library' tab in the Resource Bar and select the '2D Section Library' item and then the folder for whatever units you are wotking in. There you will find a 'Slot' profile. Just select it and drag it onto your model and you will have all the tools need to position and rotate it. Once placed you can edit it by double-clicking the curves which will take you into the sketch of the 'Slot'. Then to add the slot to the sheet metal part, simply use the 'Normal Cutout' function and select the 'Slot' profile as 'feature curves'. You will note that 'centerline' curves which can be referenced will be included in the model.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[deedub777]

And use Normal Cutout in sheet metal, this will ensure the 'cut' edges are perpendicular to the sheet faces.