Showing results for 
Search instead for 
Did you mean: 

Turbomachinery Milling with NX CAM Part 1, Setup

Community Manager Community Manager
Community Manager


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


Blisk Milling


Created with NX 7.5




Step 1 – Load the template

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.



Step 2 – Process design

Decide if:

  1. More than one roughing operation is needed. If so, you must define and use a blank in order to do efficient re-roughing in a second step. If not, you don’t need to define blank - it impacts the performance of generating the roughing operation. The fact that only ball tools are supported in this version may influence this decision. (note: NX 9 can rough turbo components with flat and bull-nosed tools.)
  2. Blades should be finished all around or leave edge(s) to be milled by a separate edge finish operation. The fact that the current version does not contain a dedicated edge finish operation may influence this decision.

Step 3 – Workpiece

In the workpiece define the following:


  • Part – the geometry in the “zone of interest”. Hub, blade, blend and splitters must be subset of Part. Selecting too many faces (i.e. – on the other side of the impeller) will impact the performance.
  • Check - any geometry that may interfere with the expected toolpath. Selecting geometry clearly outside the milling zone will impact performance. Blade, blend, hub and splitters in the milling area are considered. No need to define them as Check.

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.


  • Blank – required only if an In-Process Workpiece (IPW) consideration is needed (see step 2 above). If required, select the geometry used for turning. 



Step 4 – Blade geometry selection

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.


  • Hub – Can be single surface or patched, can be all around the Impeller or cover only a segment of it. Needs to extend at least between leading and trailing edge (Can go beyond). This face(s) must be rotary around axis of rotation.
  • Shroud – this represents the rotational face(s) covering the top of the blade. Here you can select either top face(s) of the main blade or the appropriate faces from the geometry used for turning.







  • Blade – select Blade faces without blend and top. These faces can span to the Hub, can go below it or leave a gap from it (as long as the gap between the Hub and the Blade / blend is larger than tool radius).


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:  



  • Blade Blend – specify Blend geometry. This is not a required input in the case when the geometry does not contain it, yet it is required that the radius of the used tool is larger than the expected Blend radius.
  • Splitters – through the Define Splitters dialog you can define up to 5 different Splitters.



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).


  • Number of Blades – Number of main Blades on the impeller. 


Step 5 – Operation creation

Create each operation using an appropriate template.



Make sure that the operation Geometry is set properly as the defined BLADE_GEOM.



Step 6 – Tool selection

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”  (point on face) snapping and place the tool on the Hub at the narrowest point between the Blades and / or Splitters.

select location


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.



Do you have a question?

Click 'Add a Comment' below to ask it. (You must be signed in to use this feature.)




About the Author


Holder.jpg 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.
LIVE Tech Tip Webinars
Watch NX experts demonstrate manufacturing best practices. Stay online for Q&A.