Extended modules > Advanced Machining > Types of machined features > Thread Bolt with Clearance Parameters
  
Thread Bolt with Clearance Parameters
When creating, copying, or modifying a threaded bolt with clearance, the application displays the Thread Bolt (Clearance) 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 display a graphical representation of the threaded bolt with clearance. 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 used to add the bolt to. Clicking a face automatically derives values for CenterPt and Axis Dir (provided you have not deactivated Creo Elements/Direct Machining settings).
Center Point
(CEN_PNT)
3D Position
Specifies the center point for the bolt. 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 (provided you have not deactivated Creo Elements/Direct Machining settings).
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 Creo Elements/Direct Machining settings).
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; the default is :inch if you have an imperial length unit set.
Thread Diameter
(THREAD_DIA)
Length
D1
The nominal diameter of the thread. If you specify a thread diameter smaller than the bolt diameter, a shoulder will be created. You cannot create this feature with a thread diameter larger than the bolt diameter.
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.
Bolt Diameter
(BOLT_DIA)
TolerancedLength
D2
The diameter of the bolt to be added.
Thread Length
(THREAD_LENGTH)
TolerancedLength
T1
The length of the thread.
See the Specify tolerance for further information.
Total Length
(TOTAL_LENGTH)
TolerancedLength
T3
Specifies the total length of the thread including the clearance allowed for an incomplete thread.
See the Specify tolerance for further information.
Bolt Length
(BOLT_LENGTH)
TolerancedLength
T4
Specifies the overall length of the bolt.
See the Specify tolerance for further information.
Chamfer Depth
(CHAMFER_DEPTH)
Length
T2
The depth of the front chamfer measured in direction of the axis.
Chamfer Angle
(CHAMFER_ANGLE)
Angle
The tip angle of chamfer cone.
Back Blend Rad
(BACK_BLEND_RAD)
Length
R2
The radius of the blend to be applied at the edges connecting the bolt diameter face and the face the bolt is connected to.
Shoulder Inner Blend Rad
(SHOULDER_INNER_BLEND_RAD)
Length
R1
The radius of the blend to be applied at the edge connecting the nominal diameter face (clearance) and the shoulder face of the bolt. If the nominal diameter is the same as the bolt diameter, no blend will be created and this value will be set to zero.
Dia DP
(DIA_DP)
The docuplane which should own the diameter 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 dimension, switch off the variable. You can reactivate your last value (within the same dialog box) later by switching it on again.
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, 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, 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, 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 dimension, 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.
You can enter the following parameters in the customization tables. You cannot enter these parameters as keyword value pairs at the user input line and in the Thread Bolt (Clearance) dialog box:
Dialog Field
(Keyword)
Type
Label
Description
(CHAM_DIA)
Non-negative length
An alternative method to specify the depth of the front chamfer. The chamfer diameter can be measured in the front face of the bolt.
(STD_TAP_CLEARANCE)
Positive Number
The difference between the total length and the thread length.
The remaining buttons in the dialog box 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 safety zone related input fields.
Next
(NEXT)
Completes the current operation and prompts you for the next location (create, copy) or feature (modify) without closing the menu.
As soon as the application has enough data it provides 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 bolt feature, the feature is given the status invalid. This is indicated by the label turning red. The feature is given the status invalid regardless whether the feature is still usable or not.
However, there are situations when Boolean Operations or dynamic modification functions do not really invalidate the features. In contrast to the holes created by MachiningAdvisor, the outer thread features do not have the capability of automatic verification. Thus they will stay invalid until you modify them and force the parameters to be actual.