Create Single Spot Drill Operation for Multiple Sets of Holes in NX 9

Creating a single spot drilling operation for all the holes in your part in NX 9 takes some manual interaction. The hole making operations in NX 9 read the feature information from the model to create a single spot drilling operation because of the dynamic IPW. The following step illustrate a successful work-around. However, if the steps are not taken, the spot drill operation will drill the depth from the first selected hole. Create a hole making operation in NX 9 CAM

Select the Spot Drilling sub type. (Within the create operation dialog, select your program, tool, geometry group, and machining method group). Next select your geometry. The hole should be selected at the edge of the top surface you wish to be spot drilling.

Select your hole by selecting the ICON circled in red. After selecting the Icon, this dialog box appears.

Select the first hole (Notice when selecting the hole it populates the list in the list section of the above dialog box; also if you view the graphics area inside NX 9, The dynamic IPW is displaying. The material that will be removed is displaying in the IPW).
In order to create a single spot drilling operation the next step MUST be complete.
The programmer must enter the depth manually in the above dialog box. Click on the lock to the right side of the depth value that is currently greyed out. Select the user-defined option.
Enter the depth that you wish to drill (Notice when you enter your desired spot drilling depth, the dynamic work piece automatically changes.)
This step must be done for each hole you wish to be part of your spot drilling operation. The depth of your spot drilling is derived from the surface in which the hole to be spot drilled was selected.
If a hole is selected out of order and the programmer wishes to re-order his hole, the hole must first be selected on the list. The programmer must then utilize the up and down arrows to order the hole in the proper drilling sequence.
Note: If the depth of the spot drill drills a larger chamfer than its model, NX will give a warning that the part is being gouged. Simply turn the gouge checking off. NX will also ignore drilling the holes where the gouging is occurring. This is shown in the video below. NX CAM had the intelligence to know the user was drilling a larger
spot drill and reported a gouge. Once the gouge checking is turned off in the operation, the software proceeds to drill the spot drill hole to the specified size.
To turn the gouge checking off uncheck the “Gouge Checking” option circle in the dialog box below.
Generate your tool path and select OK to accept it.
This concludes creating a single spot drilling operation with the new NX 9 hole making, spot drilling operation.
Written by Brian Brown, Application Engineer, Swoosh Technologies & Solutions
Post by Brian Brown

Leave a Reply

Your email address will not be published.