Extended modules > Advanced Machining > Types of machined features > Countersunk Through Hole Parameters
  
Countersunk Through Hole Parameters
When creating, copying, or modifying a countersunk through hole, the application displays the Countersunk Through Hole dialog box. The 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.
Use the Show Image button to display a graphical representation of the countersunk through hole. Use the Show T&Q button to add the tolerance and surface quality buttons 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).
Drill Diameter
(DRILL_DIA)
Toleranced Length
D1
Specifies the diameter of the hole to be drilled. 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).
Drill Depth
(DRILL_DEPTH)
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).
Chamfer Depth
(CHAMFER_DEPTH)
Length
T2
The depth of the chamfer measured in direction of the axis.
Chamfer Angle
(CHAMFER_ANGLE)
Angle
The tool tip angle of the sink tool.
Chamfer Depth
(BACK_CHAMFER_DEPTH)
Length
T3
The depth of the backside chamfer measured in direction of the axis.
Chamfer Angle
(BACK_CHAMFER_ANGLE)
Angle
The tool tip angle of the sink tool.
Side Surface Quality
(SIDE_SF_QUAL)
Specifies the surface quality of the side of the drilled hole.
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) later by switching it on again
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 box, 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
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.
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 menu.
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. Up front Creo Elements/Direct Modeling gets interactive after a command (that is, 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 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.