This is article 1 of a 3 part series that describes the process steps and considerations for milling a multi-bladed part using NX CAM Turbomachinery Milling.
Part 1 - Setup
Part 2 - Roughing
Part 3 - Finishing
Load from the template file the MCS. It will bring along the Part and MULTI_BLADE_GEOM:
If needed, when defining the MCS you can set a cylindrical clearance.
In the workpiece define the following:
Check geometry is not instanced. In case there are Check geometry faces / bodies attached to each blade / splitter, you must select them all.
If the trailing edge of the blade is part of one rotary face all around, this face is not part of the blade geometry, so it is recommended that you select it as a check. In some rare cases the top of the blade also needs to be selected as Check (when the shroud is not part of the blade geometry).
In some rare cases the tool needs to tilt so much that interferes with a blade beyond the milling zone (not the one bounding the milling zone). In this case it needs to be explicitly selected as Check.
Other cases where using Check is required.
In the case when Check geometry is needed locally for one operation but interferes with other operations, it should be selected from within the operation dialog.
Set the axis of rotation to follow the impeller rotary axis. Note that from now on the edge along the positive direction would be referred as leading edge regardless its functional role.
Note: the area to be rough milled is to the right side of the selected Blade (CCW around rotary axis).
Usually, the trailing edge is not included in the Blade definition. But in case the trailing edge needs to be selected as part of the Blade, but is actually part of a rotary face around the Blade as shown here...
...then you need to extract that face (if it is a solid body) and trim it so that the applicable portion of it could be selected:
Each Splitter is a combination of wall faces and blend faces. The selected Splitter should be next to the selected main Blade on its right (CCW about the axis). In the case where there are multiple Splitters between two main Blades, select them in sequence from left to right. Each Splitter should be selected separately, even if two Splitters share identical geometry to their surrounding (otherwise this can slow down tool path generation).
Create each operation using an appropriate template.
Make sure that the operation Geometry is set properly as the defined BLADE_GEOM.
Only ball end mill tools are supported. (note: starting in NX9, roughing can be done with flat or bull-nosed tools.) Define or select the required tool including its shank and holder.
With the Edit / Display dialog open, enable the “Point on Face” () snapping and place the tool on the Hub at the narrowest point between the Blades and / or Splitters.
Use the dynamic handles to place the tool in its expected milling orientation.
Based on the specified Blade Stock, Tilt Angle, Allowance for gouge prevention, and compensation for smoothing, the system attempts to use the defined tool to mill the entire part. You can specify tools that are too large to mill the whole volume, but it may be easier to use a smaller / longer tool than to specify additional operations.
Click 'Add a Comment' below to ask it. (You must be signed in to use this feature.)
|Eddy Finaro started his professional career as a mechanical engineer working with various airborne mechanical systems. He spent 8 years as an Application Engineer and Product Manager with Cimatron. Since joining Siemens PLM 5 years ago he has worked as an NX CAM Product Manager responsible for complex milling. His expertise is in 3- and 5-axis milling, particularly complex parts such as impellers, blisks, and airframe parts, etc. Eddy holds a M.Sc. degree in Aerospace Engineering. On his free time Eddy enjoys Mountain Biking, Hiking and mentoring a First Robotic Competition Team.|