Thread Milling 1

[Cam5axis]

Hi,

How to do the thread milling UG NX4 (It can be done from the top to bottom),i wanted to do thread milling from the Bottom of the part to top of part (Reverse).

Thanks

 

[joycejo]

Thread milling procedure

1. The model must have a symbolic thread feature. If not link the body and insert thread feature ( make sure you select the correct thread form! )

2. Create thread millling operation

3. On the thread milling dialog click User Parameters

4. Click Select to pick the thread geometry

5. Pick the thread feature ( the face where the thread feature is should highlight)

6. You will see two cone heads indicating the tool axis and the thread axis(direction)

7. If you want to climb mill you will have to click select start and pick the bottom dashed circle for the start of the thread. You now should have the option to reverse the thread axis.

8. You will need to define a tool for the thread. The system will give you a default too with the correct pitch. You can edit this and enter the diameter and insert length. The insert length is important! This controls the number of passes the system needs to cut the length of thread from the feature.

9. Set your feedrates for Cut , engage , retract, traverse, approach The approach feed is critical as this is the feed used when the tool travels down thru the center of the hole.

10. To get the tool to start near the center when using a helical engage

11. Set the engage and retract to helical. There is a bug here that you are limited to the length of the engage move.

12. Click machine and click cutter compensation and activate the cutcom.

13. Now you have an option for a minimum move and minimum angle. These values control the move from the approach to the engage. Tweak these values until the tool starts on or near the center of the hole.

14. You can also enter a number of passes on the machine control dialog.

15. The tool should rapid to the top of the hole and then feed at the approach feedrate to the start of the cutcom move. Engage into the cut on a helical motion. Cut the thread and then retract. Move away on the cutcom motion and then rapid out of the hole.

16. Do not use the start point under avoidance. This has a bug where the tool rapids to the start point then back to the top of the hole. It is useless and cannot be unset once it is defined.

Hope this helps


John Joyce
i Knowledge Solutions

http://www.ikstata.com