Extended modules > Advanced Machining > Types of machined features > Stepped hole > Partially Threaded Blind Hole Step Parameters
  
Partially Threaded Blind Hole Step Parameters
When creating or modifying a partially threaded blind hole step, the application displays the PartThreadBlindH dialog box. The partially threaded blind hole step parameters are described in the table below.
When using the modifying commands, the existing parameter values are loaded from the model into the dialog box where they can be edited.
Use Show Image to display a graphical representation of the partially threaded blind hole step. Use Show T&Q to add the tolerance and surface quality options to the dialog box.
Hole Dimensions
Dialog Field
(Keyword)
Type
Label
Description
TAP Units
(TAP_UNITS)
Keyword
:METRIC
:INCH
:BSW
:BSF
:BSP
:UNC
:UNF
:NPT
:PIPE_RP
:PIPE_G
:TRAPEZOID
:FLAT_TRAPEZOID
:SAW
:ROUND
:ROUND_MINING
:EDISON
:PIPE_JIS_B_0203
:PIPE_PG
:METRIC_FINE
The default is :METRIC threads, if you have a metric length unit set within Creo Elements/Direct Modeling and :INCH if you have set an imperial length unit.
ThreadDia
(THREAD_DIA)
Length
D1
The nominal diameter of the thread.
ThreadSize
(THREAD_SIZE)
Length
The pitch of the thread.
ThreadTpi
(THREAD_TPI)
Number
Alternative method to specify the pitch of the thread by entering the Thread Per Inch value for all imperial style threads and pipe threads.
Starts
(THREAD_STARTS)
Number
The number of thread starts. This value has no effect upon the geometrical representation of the threaded hole, but the data is needed for complete specification of the thread in order to create correct manufacturing documents. The default is 1.
Direction
(THREAD_HAND)
Keyword
The direction of the thread. This value has no effect upon the geometrical representation of the threaded hole, but the data is needed for complete specification of the thread in order to create correct manufacturing documents.
The following keywords are possible :
:RIGHT (the default)
:LEFT
Nom.PipeDia.
(NOMINAL_PIPE_DIA)
Length
The nominal diameter of a pipe thread, which is not the "outer" diameter of the thread. This value has no effect upon the geometrical representation of the threaded hole, but the data is needed for complete specification of the pipe thread in order to create correct manufacturing documents.
Drill Dia
(DRILL_DIA)
Length
The diameter of the hole to be drilled.
Tap
Depth
(TAP_DEPTH)
Toleranced Length
T2
The depth of the thread.
If you have added a tolerance to this parameter through the Creo Elements/Direct Annotation 3D module or by direct specification within the dialog box, it is written into the output file to be transferred to the receiving CAM system (in either ISO or values). See the Description about specifying the Tolerance of a length value for further information.
Normally, the tap depth (a parameter) is derived from the thread diameter and set to a default value by the system (Creo Elements/Direct Modeling). The value is slaved to the drill depth, unless explicitly set.
* 
To set the tap depth value:
• Type the value in the Tap Depth box and press ENTER or,
• Click the Tap Depth box to accept the actual value (to activate the parameter) and then press ENTER.
If the drill depth is changed when still slaved to the tap depth, the tap depth is recalculated again by subtracting the standard tap clearance from the drill depth.
DrillDepth
(DRILL_DEPTH)
Toleranced Length
T1
Specifies the drilling depth. The depth is defined as the length of the drilled cylinder and does not include the tip of the drill tool.
If you have added a tolerance to this parameter through the Creo Elements/Direct Annotation 3D module or by direct specification within the dialog box, it is written into the output file to be transferred to the receiving CAM system (in either ISO or values). See the Description about specifying the Tolerance of a length value for further information. See also Meas Mode.
Normally, the drill depth is derived from the thread diameter and the hidden customization value, standard tap clearance (STD_TAP_CLEARANCE). The drill depth (a parameter) is set to a default value by the system (Creo Elements/Direct Modeling). The value is slaved to the tap depth, unless explicitly set.
* 
To set the drill depth value:
• Type a new value in the DrillDepth box and press ENTER or,
• Click the DrillDepth box to accept the actual value (to activate the parameter) and then press ENTER.
If the tap depth is changed when still slaved to the drill depth, the drill depth is recalculated again by adding the standard tap clearance to the tap depth.
Cone Angle
(CONE_ANGLE)
Angle
A1
The tip angle of the drill tool to be used for the drilling operation. A 118 degree default is used. The following restrictions apply: 0 < A1 <= 180 degree, that is, you can create a flat blind hole, but there are special commands to do so (simply replace the BLINDHOLE by FLAT_BLINDHOLE in the name of the command).
Cham Depth
(CHAMFER_DEPTH)
Length
T3
The depth of the chamfer measured in the direction of the axis.
Cham.Angle
(CHAMFER_ANGLE)
Angle
The tool tip angle of the sink tool.
You can enter the following parameters as keyword value pairs at the user input line or in the customization tables:
Dialog Field
(Keyword)
Type
Label
Description
ThreadTpi Numerator
(THREAD_TPI_NUM)
Non-negative Number
The numerator part of a rational thread per inch value for the thread pitch. This parameter is applicable to :NPT and :UNC type threads. For other type of threads, if a positive value occurs in a customization table, then the numerator value is forced to zero.
ThreadTpi Denominator
(THREAD_TPI_DEN)
Positive Number
The denominator part of a rational thread per inch value for the thread pitch. This parameter is applicable to: NPT and :UNC type threads. For other type of threads, if the value in a customization table is greater than one, then the denominator value is forced to one.
The following parameter can neither be entered as a keyword value pair in the user input line nor set using the graphical user interface. This parameter can only be used within customization tables.
Dialog Field
(Keyword)
Type
Label
Description
(STD_TAP_CLEARANCE)
Positive Number
The difference between the drill depth and the tap depth.
The remaining options in the dialog box do the following:
Dialog Field
(Keyword)
Description
Show/Hide Image
(IMAGE_SHOWN)
Shows or hides the graphical representation of the machined hole.
Show/Hide Tolerance & Quality
(TOLERANCE_AND_QUALITY)
Shows or hides additional tolerance-related input fields.
As soon as the application has enough data it provides a graphical feedback to outline the size of the feature being defined. This feedback is updated with every new parameter. Normally, feedback is displayed as soon as a face is selected and a diameter is specified.