Cancel
Showing results for 
Search instead for 
Did you mean: 

Turbomachinery Milling with NX CAM Part 2, Roughing

Community Manager Community Manager
Community Manager

Overview

This is article 2 of a 3 part series that describes the 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

 

Details

 

Step 1 – Specify the stock

On the cutting parameters dialog open the ‘Stock’ tab and key in the blade and hub stocks:

  • Blade stock– stock to leave on the blades, blends and splitter(s).
  • Hub stock – stock to leave on the hub.

 

Step 2 – Specify the drive method

  • Set the Cut Pattern: Zig / Zig Zag with Lifts.
  • Set the Stepover. Note that this is a maximum value based on the largest distance between outer passes. Increasing the extensions may add milling passes.
  • Specify Start Point – select between the 6 arrows on the graphic area:

 

drive method start point

 

  • Set the Cut Direction. Note that the available cut direction options are sensitive to the selections done for Cut Pattern and for Start Point.

Press the “Display” button to generate the preview. Note that preview requires the operation to have the tool defined and all geometries selected. With Cut Levels set to "offsets from shroud" the preview is displayed on the shroud level since most likely the hub level is trimmed and doesn’t represent the real milling pattern.

 

Estimate the results: Note that the preview seen here is influenced also by definitions done in other dialogs, yet it provides a good feedback to define the controls included here.

 

Trimmed tool path means the tool cannot fit in at all regions.

trimmed path

 

To avoid that you may want to do one or more of the following changes:

  • Tool Axis dialog – change “Rotate about” option  “Part axis” to “Blade” and / or decrease the tilt clearance angle.
  • Cutting Parameters dialog – decrease Blade Stock, decrease Part Safe Clearance, change the Axis Smoothing % and the Max Blade Roll Angle.
  • Change tool and / or cut levels.

“Crossing paths” are not necessarily bad. Remember that the tool path displays tool tips, but the contact point moves around depending on tool tilting. The tool tip locations may cross each other while the contact points with the hub are as expected.

 

crossing paths

 

Based on the blank material knowledge set the Tangential Extensions and Radial Extensions to provide full coverage.

 

extensions1

Tangential Extension = 50%Tool; Radial Extension = 0% tool

 

extensions2

Tangential Extension = 100%Tool; Radial Extension = 100% tool

 

Note not to set values larger than needed for each.

 

You can control the snip point, which determines where the cutting motions driven by the surrounding blades end and the extensions start. The default “Blade Edge Point” is set to “Along Blade Direction” which is appropriate for most cases. To get further control it can be changed to “Along Part Axis” which requires also a “Distance” setting. Different options are (crudely :-) sketched in the following images:

 

along blade direction

Along Blade Direction

 

along part axis

Along Part Axis, Distance = 0

 

along part axis

Along Part Axis, Distance = D

 

Blade Edge Point” definition is common to the leading and trailing edges, however, in case of “Along Part Axis” the “Distance” can be set apart for the trailing edge and for the leading edge. Same value is used for the right side and for the left side.

 

Step 3 – Specify the Cut Levels

When invoking this dialog you can immediately see the expected cut levels spacing as triangles dynamic preview.

 

Set the required depth mode:

  • Offsets from hub - each cut level is created on constant offset surface patch from the hub. In this case the depth of cut is constant

offsets from hub

 

  • Offsets from shroud - each cut level is created on constant offset surface patch from the shroud. In this case the depth of cut is constant as the lower cut levels reach the hub, the passes are not trimmed, but rather extended along the hub to perform passes connections outside the impeller.

offsets from shroud

 

  • Interpolate from shroud to hub – The hub level and the shroud level are interpolated to determine intermediate cut levels. In this case the depth of cut varies along the pass.

 interpolate from shroud to hub

 

Set the Range Depth.

  • Automatic would span the cut levels across the whole depth to be milled, while Specify allows you to determine the number of cuts to be milled.
  • For Offsets From Hub or Offsets From Shroud the system will generate the specified number of cuts spaced by the depth per cut distance, while for Interpolate From Shroud to Hub the given number of cuts is equally spaced across the whole depth to be milled.
  • For interpolate from shroud to hub the user can limit the cut volume by changing the Start % (highest cut level) and the End % (Lowest cut level).

 

Press the Display button to generate the preview. The preview here shows the cut levels as distributed along the blades and splitter(s). Change parameters as needed to get proper results previewed. Note that this preview also shows the passes extensions on the higher cut levels, so you may want to switch to the drive method dialog to fine tune some parameters there.

 

Step 4 – Specify the tool axis orientation

The tool axis orientation is controlled by the settings in the Automatic Tool Axis Orientation dialog and the Tool Axis Control tab of the cutting parameters.

 

In the Automatic Tool Axis Orientation dialog:

Tilt Clearance Angle - controls the minimal allowed deviation between the tool and the blades / splitters:

 

tilt angle 0 

Tilt Angle = 0 deg

 

tilt angle 10 

Tilt Angle = 10 deg

 

Lead / Lag Angle at Leading and Trailing Edges - can be used to prevent heal digging. In case of Zig Zag, inclination changes with direction change. “Rotate About” controls the method the operation uses to tilt away from potential collisions. Rotation About Part Axis uses the part axis as base for tilting. Rotation About Blade uses the pass direction as the rotation axis. Rotation About Part Axis is expected to provide a steadier tool axis behavior, while the Rotation About Blade is expected to succeed in case of tight conditions and blades highly twisted around the part axis. 

 

In the Tool Axis Control tab of the Cutting Parameters dialog:

Maximum Blade Roll Angle - controls how much can the tool be tilted attempting to lean toward the blade.  

 

max blade roll angle 30

Maximum Blade Roll Angle = 30 deg

 

max blade roll angle 0

Maximum Blade Roll Angle = 0 deg

 

Note that reducing this value prevents the tool from leaning towards the blade:

 max blade roll angle 30

Maximum Blade Roll Angle = 30 deg

 

max blade roll angle 0

Maximum Blade Roll Angle = 0 deg

 

 

Step 5 – Other Cutting Parameters

 

Path Smoothing % - this controls the smoothing of the passes ahead of splitters leading edge. The Smoothing slider smooths out the orientation changes. Note that for some cases high Smoothing% may prevent the system from finding gouge free orientation (this will trim the cutting motions). With some special geometries, as the tool approaches the edge it may be tilted to excessive orientations without real need. User can set a Distance From the Edge where the tool orientation will freeze and be reused for rest of the segment to the edge.

 

path smoothing 0

Path Smoothing %= 0

 

path smoothing 30

Path Smoothing %= 30

 

Blank Stock– inflates the blank or the IPW.

Shroud Stock – offsets the shroud to control the higher cut levels. Negative value causes the highest cut level to start deeper below the shroud. Positive values are not supported initially, but when implemented will add cut levels above the shroud.

Blade Stock and Hub Stock– minimum allowed remaining stocks on the blade and hub respectively. Blade Stock value is used for all blades, blade blends, splitters, blend splitters and check geometries. In some cases where the outer passes are hazy set Blade StockHub Stock.

Part Safe Clearance – set additional clearance from the holder to the part and check geometries. Note the in case of tight geometries this value should be minimized. This is especially true for cases where a portion of the tool is described as holder (i.e. the cylindrical portion of a taper tool).

 

Step 6 – Blank consideration

If blank was defined in one of the geometry groups the operation inherits from it will be considered. That means the same motions are initially calculated, but all motions where the tool is not touching the blank are trimmed. Non-Cutting Moves (NCMs) are used to connect across the gaps. In the Cutting Parameters dialog user can select to consider 3D IPW instead of Initial Blank. That means that an internal simulation is used to calculate the IPW state after all previous operations milled the initial blank. In this case the user can further control: Minimum Material Removed, Hookup Distance, and Minimum Cut Length – a cutting motion smaller than this values is neglected

 

This is also the order these parameters are considered (so small gaps are hooked up before removing small segments). Blank consideration is optional. In the classic case where the blank is initially turned to the shroud level, having the blank defined will increase the generation time without changing the result. Blank is needed only if one of the next operations uses 3D IPW consideration. IPW calculation is time consuming. To save time on next regenerations it is recommended to set “Save IPW Model” in the Manufacturing Preferences / Geometry / In Process Porkpiece menu.

 

Step 7 – Non Cutting Motions (NCMs)

All Non Cutting Motions options and controls are identical to rest of the operations. Every connection between leading and trailing edges is considered “Between Region.” Connections from one cut level to the next is controlled by the Region Distance as long as it is done on the same edge. A new option “Smooth” traverse type was added in NX 7.5. Though available for all operations, it is very effective using it with the family of these of operations.

 

Step 8 – First cut feed rate First pass at each cut level is a slotting pass.

In the Feeds and Speeds dialog the user can set a slower First Cut feed rate for this slotting motion. In case one or more splitters exist, the first pass at each segment is controlled by the First Cut feed rate. Visualize these first cuts using the Edit Display / Path Display Colors and set the color of the First Cut motions to be different than the Cut motions.

 

Step 9 - Generation results assessment

After generation use the Verify Tool Path tool path verification  to assess the results. Being a cut level-based operation it is recommended to use the ‘Current Level’ display, and to check the ‘Pause at Each Level’.

 

tool path verification dialog

 

This way you can navigate between levels using the tool path verification controls buttons.

 

Visualize the tool path to see if all levels are completely cut, if changes to the extensions or other controls need to be done. Visualize the tool motions to see if tool axis control parameters are set properly. Additionally, the Operation Navigator provides Gouge Check capabilities as a MB3 option for the operation.

 

 

Step 10 - Instancing

Programmers are expected to program the these cuts just once, for a single blade/splitter sequence. Tool paths are then re-used, or "instanced" around the hub as needed. There are a few ways to accomplish this:

  • Using the Operation NavigatorObject / Transform for this operation
  • Let the post processor process the operations as Macros. NX outputs the macro code needed for this as part of these operation types, so the post can make the "define as Macro" code, followed by the several "use Macro" codes.
  • Output the G-code once and then manipulate instances using the controller. For example the operator could simply index a rotary axis and rerun the cuts as needed.  This is the most manual method.

 

In the case that the machinists desire to cut in a sequence that roughs, then finishes one level at a time before roughing deeper (sometimes a requirement for thin blades), the instancing of these operations needs to account for this sequence preference. These operations are level-based, and so have a level marker at each level. This enables the post to process these where N levels are cut at once, than in the next instance same N levels are cut and so on till N levels are cut all around. Than next N levels are cut in the first instance and so on. (Note that NX 9 includes specific support for cutting these kinds of rough/finish sequences without resorting to such post processor gymnastics.)

 

Hub Finish

Hub Finish is actually the lowest cut level out of the rouging operation, so all steps described for the roughing are identical for the Hub Finish excepting step 3 – cut levels and step 6 – blank consideration. Also, Hub Finish does not require shroud geometry as input. Hub Finish covers only the hub and not the blends. In case opposing blends touch (overlap) each not leaving space for the hub, this portion will not be finished and non-cutting moves (NCMs) will connect the gap.

 

 

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.