Threaded Holes

The Thread capability removes material surrounding the hole. To define a thread, you can enter the values of your choice, but you can use standard values or personal values available in files too. 

This task shows you how to create a threaded hole using values previously defined in a file. 
Open the Hole1.CATPart document.
1.  Click the Hole icon . 
2.  Select the face on which you wish to create the hole.

3. In the Hole Definition dialog box that displays, define the hole shape and enter the parameters of your choice. For more information, refer to Hole.
  4. 

Click the Thread tab.
  5.

Check Threaded to access the thread definition options.
 
  You can define three different thread types:
No Standard: uses values entered by the user
Metric Thin Pitch: uses AFNOR standard values 
Metric Thick Pitch: uses AFNOR standard values
 
Metric Thin Pitch: AFNOR standard
 

Refer to (NF E03-053-1970). This normative reference is linked to  NF E03-051-1982) 

The application uses the minimum standard values. 
 
Nominaldiam        Pitch Minordiam M
8.0 1.0 6.917  
9.1 1.0 7.917  
10.0 1.25 8.647  
12. 1.25 10.647  
14.0 1.5 12.376  
16.0 1.5 14.376  
18.0 1.5 16.376  
20.0 1.5 18.376  
22.0 1.5 20.376  
24.0 2.0 21.835  
27.0 2.0 24.835  
30.0 2.0 27.835  
33.0 2.0 30.835  
36.0 3.0 32.752  
39.0 3.0 35.752  

 
 
Metric Thick Pitch: AFNOR standard

Refer to (NF E03-053-1970). This normative reference is linked to  NF E03-051-1982) 

The application uses the minimum standard values. 
 

Nominaldiam 

 Pitch Minordiam M
1 0.25 0.729  
1.1 0.25 0.829  
1.2 0.25 0.829  
1.4 0.3 1.075  
1.6 0.35 1.221  
1.8 0.35 1.221  
2.0 0.4 1.567  
2.2 0.45 1.713  
2.5 0.45 2.013  
3.0 0.5 2.459  
3.5 0.6 2.850  
4.0 0.7 3.242  
4.5 0.75 3.688  
5.0 0.8 4.134  
6.0 1.0 4.917  
7.0 1.0 5.917  
8.0 1.25 6.647  
9.0 1.25 7.647  
10.0 1.5 8.376  
12.0 1.75 10.106  
14.0 2.0 11.835  
16.0 2.0 13.835  
18.0 2.5 15.294  
20.0 2.5 17.294  
22.0 2.5 19.294  
24.0 3.0 20.752  
27.0 3.0 23.752  
30.0 3.5 26.211  
33.0 3.5 29.211  
36.0 4.0 31.670  
39.0 4.0 34.670  
42.0 4.5 37.129  
45.0 4.5 40.129  
48.0 5.0 42.587  
52.0 5.0 46.587  
56.0 5.5 50.046  
60.0 5.5 54.046  
64.0 6.0 57.505  
68.0 6.0 61.505  
72.0 6.0 65.505  
76.0 6.0 69.505  
80.0 6.0 73.505  
85.0 6.0 78.505  
90.0 6.0 83.505  

 
  6. Keep the option No Standard.
  7. As you wish to use values already defined in an file, click Add to access this file. Otherwise, you could directly enter values in the fields.

A dialog box displays, in which you can navigate to reach the file containing your own values. This file may be of one of the following types: 
Excel files (general format)
Lotus files
tabulated files (in Unix environment)
 
  8. Navigate to STANDARD1.txt  file and click Open to get the values it contains. 

The Hole Definition dialog box reappears.

Your file was created as follows:

Nominal diameter Pitch Minor Diameter Key
the first row contains no numerical values
the other rows below are reserved for numerical values
the mandatory items are keys that define the names associated with the values.

Moreover, the name of the standard is the same as the name of the file without the extension.

Remember these recommendations for creating your own personal files. 
  9. Set the Type option to STANDARD1.
  10. Define the nominal diameter: set the Thread Diameter to a value. For example, set USR1.9.

You can note that the Hole diameter as well as the Pitch values are then provided in the corresponding fields.  The Pitch field  defines the distance between each crest.
 

  11. If necessary, edit the Hole Diameter value if you need to modify the value you had previously set in the Extension tab. This value must not exceed the thread diameter value.
  12. Repeat the operation for editing the thread depth if necessary too.
  13. Check the Left-Threaded option.
  14. Click OK to confirm your operation and close the Hole Definition dialog box.
  The application displays the hole in the geometry area but not the thread. Note also that an icon specific to this feature is displayed in the specification tree.
 

A Few Words About Removing Files
  The Remove button removes files containing user-defined values. You cannot remove files containing standard values. Clicking the Remove button displays the list of user-defined files. You then just need to select or multi-select  (using ctrl key) the files and click OK to confirm the operation.
 

  Note also that you cannot remove a standard file if it is used for a hole created in the CATPart document.
 
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