Cancel
Showing results for 
Search instead for 
Did you mean: 

THREADED HOLES PARAMETRIC PART

Valued Contributor
Valued Contributor

HI EVERYONE,

 

I HAVE TO DO A QUITE COMPLICATE PARAMETRIZED PART, WICH WILL TURN INTO A STANDARD PART O A FAMILY PART.

 

THING IS, I HAVE MANY EXPRESSIONS DEFINING MY PART, BUT I AM NOT QUITE SURE HOW TO  "DEFINE" IT´ S EXPRESSION´S THREADS IN ORDER TO MANIPULATE THEM WHEN ADDING IT FROM THE LIBRARY.

 

FOR EXAMPLE, IMAGINE I WANT A STANDARD PART DEFINED AS A CYLINDER WITH A THERAD AT THE TOP ,  2 EXPRESSION DEFINE ITS HEIGHT AND DIAMETER. AND I WANT ANOTHER (OR MORE  THAN ONE...) THAT DEFINES ITS THREAD WHEN INSERTED AS STANDARD.

 

HOW CAN I DO THIS?

 

THANKS IN ADVANCE

 

MR

6 REPLIES

Re: THREADED HOLES PARAMETRIC PART

Siemens Phenom Siemens Phenom
Siemens Phenom

When creating a Threaded Hole, there are 'string' expressions created which actually control the size of the thread feature.  In the picture below, the highlighted expression, 'p96', when edited (using the value of a legitimate thread size) will cause the threaded hole to update.  If you need to change the 'Thread Standard', such as from 'Course' to 'Fine', you would also need to edit the value of expression 'p98' in my example.

 

Threaded Expression.PNG

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA

Re: THREADED HOLES PARAMETRIC PART

Valued Contributor
Valued Contributor

Hi John,

 

Thanks for reply. So I could add user defined expresion (String) ,with a legitimate thread size.

 

That string could content 2 expressions, one for thread and one for pitch. So once the part is inserted as standard, I could set thread and pitch (of course both values must define a legitime one). I think this could help avoid wrong "spelling" threads. Don´t you?

 

Thanks again!

Re: THREADED HOLES PARAMETRIC PART

Siemens Phenom Siemens Phenom
Siemens Phenom

In a situation like that, you can also create a 'List' Attribute which contains only the thread sizes that you would be using and then link the Thread Size Expression to the value of this Attribute.  Then all that you need to do to change the thread size is to pick a different attribute from the list and hit OK, as shown in the image below.  Note that these 'List' attributes are set up by going to...

 

File -> Utilities -> Attribute Templates...

 

Thread by Attribute.png

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA

Re: THREADED HOLES PARAMETRIC PART

Valued Contributor
Valued Contributor

HI John,

 

Great idea! I´ve never tried "list attributes", but I will. Is this list same kind of "expressions lists"?

Could I try to make this list in expressions dialog box? (jus to have everithing under control from expressions).

 

I will let you know how I do with this list (or contact again to ask for help to use them! he he he)

 

Thanks again John!

 

MR

Re: THREADED HOLES PARAMETRIC PART

Siemens Phenom Siemens Phenom
Siemens Phenom

These are different concepts, but you could use a 'List' expression and then just select from the list members using the 'nth' command.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA

Re: THREADED HOLES PARAMETRIC PART

sorry to necro this old thread but, what if u want to have 2 diferent threads on the same part ?

imagine in a SHCS of HASCO i want to insert a thread on the clearance with the above metric of the thread inserted

how can i define the 2nd thread ? because if i just insert the face property it will appear with the same thread as the shcs

NX 9 - 10 - 11 - 12 - MW - Journaling || vegetagaru @ engtips