Extended modules > Advanced Machining > Types of machined features > Partially Threaded Blind Hole Parameters
  
Partially Threaded Blind Hole Parameters
When creating, copying, or modifying a partially threaded blind hole, the application displays the Partially Threaded Blind Hole dialog box. These dialog box parameters are described in the table below.
When using the modifying commands, the existing values are loaded from the model into the dialog fields where they can be edited.
Click Show Image to display a graphical representation of the partially threaded blind hole. Click Show T&Q to add the tolerance and surface quality data entry fields to the dialog box.
Dialog Field
(Keyword)
Type
Label
Description
Face
(SEL_FACE)
Specifies the face for the drilling operation. Clicking a face automatically derives values for CenterPt and Axis Dir (providing you have not deactivated automatic parameter acquisition).
Center Point
(CEN_PNT)
3D Position
Specifies the center point for the drilling operation. If the starting face is deleted later by other machining operations, the center point may be left hanging in space. If you click Face and click a point on a face, the center point is derived from this point (providing you have not deactivated automatic parameter acquisition).
Axis
(AXIS)
3D Axis (Direction + Position + Up-Direction)
Specifies the axis for the machined hole. If the starting face is deleted later by other machining operations, the center point may be left hanging in space. If you click Face and click a point on a face, the axis is derived normal to this point (providing you have not deactivated automatic parameter acquisition).
TAP Units
(TAP_UNITS)
Keyword
Currently, the following threads are supported :
: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.
Thread Diameter
(THREAD_DIA)
Length
D1
The nominal diameter of the thread.
Thread Pitch
(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 Diameter
(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).
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.
Drill Depth
(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, it is written into the output file to be transferred to the receiving CAM system (in either ISO or values).
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. i.e. 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)
Chamfer Depth
(CHAMFER_DEPTH)
Length
T3
The depth of the chamfer measured in direction of the axis.
Chamfer Angle
(CHAMFER_ANGLE)
Angle
The tool tip angle of the sink tool.
Name
(NAME)
String
Specifies the name of the new feature. In case of modify this name is fixed, to modify the name of a feature please use rename.
Flag DP
(FLAG_DP)
The docuplane which should own the flag text.
If you switch on the variable for the first time within a dialog box, the computed defaults will be activated.
If you decide not to use the docuplane for the flag text but want to get a free flag text, simply switch off the variable. You can reactivate your last value (within the same dialog box) later by switching it on again
Depth DP
(DEPTH_DP)
The docuplane which should own the depth related dimensions.
If you switch on the variable for the first time within a dialog, the computed defaults will be activated.
If you decide not to use the docuplane for the dimensions but want to get a free dimensions, simply switch off the variable. You can reactivate your last value (within the same dialog box) later by switching it on again
DriDeSfty
(DRILL_DEPTH_SAFETY_ZONE_THICKNESS)
Length
The thickness of the depth related safety zone (i.e. the wall thickness of the conical tip)
If you decide not to use the safety zone, simply switch off the variable. You can reactivate your last value (within the same dialog box) later by switching it on again.
DiaSfty
(DRILL_DIA_SAFETY_ZONE_THICKNESS)
Length
The thickness of the diameter related safety zone (that is, the wall thickness of the "pipe" around the hole)
If you decide not to use the safety zone, simply switch off the variable. You can reactivate your last value (within the same dialog box) later by switching it on again.
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
(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.
(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 parameters can neither be entered by keyword value pairs on the command line (User Input Area) nor through the graphical User Interface, they can be used within customization tables only"
Dialog Field
(Keyword)
Type
Label
Description
(CHAM_DIA)
Non-negative length
An alternative method to specify the depth of the front chamfer. If the
SEL_FACE face is in a plane that is perpendicular to the axis of the hole, then the chamfer radius is the half of the hole diameter.
(STD_TAP_CLEARANCE)
Positive Number
The difference between the drill depth and the tap depth.
The remaining buttons in the menu do the following:
Dialog Field
(Keyword)
Description
Show/Hide Image
(IMAGE_SHOWN)
Shows/hides the graphical representation of the machined hole.
Show/Hide Tolerance & Quality
(TOLERANCE_AND_QUALITY)
Shows/hides additional tolerance-related input fields.
Next
(NEXT)
Completes the current operation and prompts you for the next location (create, copy) or feature (modify) without closing the dialog box.
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 from the moment a face is selected and a diameter is given.
Dynamic Modification Behavior
If a dynamic modify operation (such as the Offset command in the Modify 3D group on the Modeling tab) interferes with a machined hole feature, the feature is given the status invalid. This is indicated by the label turning red (see the following graphic). The feature is given the status invalid regardless whether the feature is still usable or not.
Top Holes Rendered Invalid
However, there are situations when Boolean Operations or dynamic modification functions do not really in-validate the features. Upfront Creo Elements/Direct Modeling gets interactive after a command (i.e. waits for commands given by the user) it checks whether features invalidated during the last command can be revalidated. It doesn't check previously invalidated features whether they can be re-validated because the obstacle has been removed The revalidation buttons Single and Multiple allow manual revalidation of features on a per feature basis. This calls a feature-specific verification-routine which checks whether the feature is still valid.
Revalidation is possible after the following operations:
• Changing the depth of the hole (via MoveFace)
• Drilling holes through the hole at an angle to the axis of the hole
• Changing the parameters of the chamfer in type, depth or angle.
• Removing the chamfer.
• Cutting away parts of the hole in a way that the cylinder is not closed anymore, i.e. the feature is still a valid one if you are punching a keyed slot into it.
• You may cut the hole into two by drilling a larger hole through it or by punching another shape through it.
• Changing the axis of the hole (via MoveFace)
Revalidation is not possible after the following operations :
• Changing the diameter of the pilot hole (via ChangeHole)
• Changing the diameter of the threaded hole (via ChangeHole)
• Changing the drilled cylinder to something else (for example, using Taper in the Engineering group on the Modeling tab or anisotropic scale)
• Changing the diameter of a part of a hole, if you have cut it into two or more sections.
Currently, you do not need to worry about revalidation of the features as the export process checks for validity and only transfers valid features. Invalid features are skipped.