Cancel
Showing results for 
Search instead for 
Did you mean: 

Turbomachinery Milling with NX CAM Part 3, Blade Finishing

Community Manager Community Manager
Community Manager

Overview

This is article 3 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

 

Blade finishing

Blade finish shares some aspects with the Multi blade roughing (see part 2 of this series): Stocks, Cut levels, Tool axis orientation (beside “Rotate about” control). The different aspects are detailed below.

 

Step 1 - Specify the Drive Method settings:

  • Geometry to Finish – Here the user selects between (main) blade, splitter 1, splitter 2, etc. (splitters available according to the geometries defined.
  • Sides to Cut – here the user selects which sides of the blade are to be finished. The sides are determined using the Snip Points, so regardless if the blade is made of one surface going all around or many surfaces, the user can still control the sides to cut.
  • In case the trailing edge was not selected as part of the blade geometry do not use the option “All Sides” to avoid gouging it.
  • Leading and trailing edges are controlled similar to the Roughing operation. Availability of the controls depends on the “Sides to Cut” selected.
  • The Blade Finish operation does not use the graphical selection of the start point. Instead the user controls the “Cut Pattern”,Cut Direction” and “Start Point” from the dialog. Availability of controls here also depends on the “Sides to Cut” selected, as well as previous Drive Method settings selected.
  • Blade Finish does not provide extensions. Use Non-Cutting Moves instead.
  • Helical tool path is not available yet. It is planned to be added in a short while. (Update: added in NX8.5)

 

Step 2 - Specify other cutting parameters:
  • Many of the controls such as “Path Soothing %” and “Blank Consideration” are irrelevant.
  • Relevant parameters have identical usage as in the roughing operation.

 

Step 3 - Other considerations:
  • Blade Finish covers the blade and blend geometries down to the hub.
  • Sometimes it is required to use a large diameter tool to finish the upper portion of the blade and a smaller diameter tool to finish the blends. It can be done in two operations where each uses a different tool and depth of cut. Both would use “Interpolated from Shroud to Hub” as the “Depth Mode” but “Start %” and “End %” are different. i.e. first works 0-85% and second 80-100%. In this case the region 80-85% is covered by both operations to provide overlapping. Static and dynamic previews help to set required percentages for the first operation.

 

Blend finishing

Blend Finishing shares some aspects with the blade finish: Stocks, Tool axis orientation. The different aspects are detailed below.

 

Step 1 - Specify Drive Method settings:
  • Geometry to Finish – Here the user selects between (main) blade Blend, splitter 1 Blend, splitter 2 Blend, etc. (splitter Blends are available according to the geometries defined).
  • Sides to cut – here the user selects which sides of the blend are to be finished. The sides are determined using the Snip Points, so regardless if the blade is made of one surface going all around or many surfaces, the user can still control the Sides to Cut.
  • In case the trailing edge was not selected as part of the blade geometry do not use the option “All Sides” to avoid gouging it.
  • Leading and trailing edges are controlled similar as for the Blade finish operation.
  • Availability of the controls depends on the “Sides to Cut” selected.

The range of the step over’s is defined by two parameters:

 

Step 2 - Specify Drive method:
  • Lower Blend Edge – use the Lower Blend Edge or the Dual Contact Pass as reference.
  • Reference Tool – user sets the diameter of the ball tool used to finish the blade and hub. Moreover, he can add overlap on hub and overlap on blade.
Step 3 - Specify Cut Band:
  • Offsets - Based on the distances on hub and on blade the Max Stepover is used to calculate the amount of passes that will equally distributed along the cut.
  • Stepovers – the user specifies number of stepovers on the hub and number of stepovers on the blade. Note that 0 on hub and 0 on blade means only 1 ‘pencil pass’ is generated.
  • The Blend Finish operation does not use the graphical selection of the start point. Instead the user controls the “Cut Pattern”, “Cut Direction” and “Start Point” from the dialog. Availability of controls here also depends on the “Sides to Cut” selected, as well as previous Drive settings selected.
  • Sequencing provides all options as found also in 3 axis flow cut operations: ‘Inside-Out’; ‘Outside-In’; ‘Steep Last’; Steep First’; ‘Inside-Out Alternate’; ‘Outside-In Alternate’.
  • Blade Finish does not provide extensions. Use Non-Cutting Moves instead.
  • Helical tool path is not available yet. It is planned to be added in a short while.  (Update: added in NX8.5)
Step 4 - Specify Other cutting parameters:
  • Many of the controls such as “Path Soothing %” and “Blank Consideration” are irrelevant.
  • Relevant parameters have identical usage as in the roughing operation.

 

Special Topic – Interpolated Tool Axis Orientation

The default method of ‘Automatic’ tool axis provides quick and good gouge free smooth orientations along the tool path. However, to get smoother results as well as to avoid cases where the ‘Automatic’ method fails to locate gouge free orientation (hence tool path is trimmed and reconnected by NCMs) in NX7.5.2 we offer a new method “Interpolated Vector”.

 

Since this option is in preview state in 7.5.2 you will need to set a new ENV: UGII_CAM_5AXIS_BLADE_FINISH_INTERP with the value 1. (Update: this feature is no longer preview as of NX8.) Limitations in 7.5.2 are detailed at the end of this section

 

The concept here is that the user can set the tool alignment along the lowest cut level and those alignments are reused for the upper cut levels in a parametric manner.

 

After defining the geometry, stocks and tool, change the Tool Axis orientation to ‘Interpolated Vector’:

interpolated vector

 

The system will spend some time to generate the lower rail along which you can define the orientations and the system points defined by a yellow arrow:

vectors

 

In case the geometry is not contiguous or tool not defined you may get some warnings / error messages same as during tool path generation.

 

You will also get the Interpolated Vector dialog:

interpolate vector dialog

 

There are a few activities you can do at this stage:

 

Display preview of tools along lower rail
  • Click the display Preview button:

preview

 

  • You will get tools displayed at interpolated locations and orientations according to settings in the list:

preview display

 

  • Those tools are colored green for safe positions or red for gouging positions. Those settings are controlled by User preferences.
  • To clear those images – refresh the screen (use refresh command or F5)

 

Change orientation of that tool at system points
  • Select one of the arrows on the screen or from the list in the dialog. You will get the tool displayed at that point and a dynamic CSYS. 
  • Grab one of the rotary handles and rotate the tool to the required position:

interpolated vectors

  • You can also enter the angle or change the dynamic snap angle from the GUIF (key-in box that accompanies interactive handles)
  •  In order to copy the initial orientation from another point right click on the other point and select “Use This Orientation

orientation

 

  • At any time you can reset to default the orientation of a point.
  •  System points cannot be deleted or moved.

 

Add, reorient, Move, delete User points
  • To add a point press the “Add New Set” on the dialog and select any point along the rail.

add new set

 

  • The point was added to the list and you can change its orientation using all options described for system points.
  • User points can be moved to any other point along the rail. Any attempt to place it off the rail will snap it to the closest point on the rail.
  • To remove a user point select it and either press the X button near the list or right click on the arrow and select “Remove”. 

remove

 

While rotating a vector, system can dynamically show the impact of the action on closest locations (including gouge check).

  • To do so check the Preview checkbox in the dialog:

preview

 

  • Result:

preview result

 

To remove this dynamic preview – uncheck the checkbox.

 

Display Interpolated vectors along the lower rail:

interpolated vectors

 

To clear those vectors – refresh the screen (use refresh command or F5).

 

Tilt Clearance Angle is not active in NX7.5.2.

clearance angle

 

In NX8 it will provide same safety clearance from the part as in Automatic tool axis.

 

Reset to Default from the dialog will delete all user points and will reset all system points to the default orientation.

reset to default

 

When copying an operation to another file or copying it to be used for a different blade / splitter in the current file it is recommended to use it to avoid applying irrelevant settings.

 

The list in the dialog contains all points. For each point it shows:

dialog

  • Whether it is system or user point
  • Its U parameter (parametric location along the rail)
  • Number of rail (in 7.5.2 only one rail is available)
  • Tool orientation at that point in terms of i, j, k. 

 

Suggested user workflow:

1. Check the Preview checkbox.

2. After invoking the Interpolated Vector dialog press the display Preview.

3. Based on red tools decide where you want to locally manipulate the orientations. Select an existing point or add a new one.

4. Press F5 to clear the screen from the static preview.

5. Rotate the tool at that point till you get it and its nearest instances collision free.

6. Press the display Preview again and see where the next location that needs manipulation is and continue this way till you get the expected alignments all over.  Note that sometimes you may manipulate orientations to minimize tool axis changes. For that you can Copy Orientation from previous / next point.

7. Press OK in the dialog and Generate the operation. On the lowest cut your tool path is most likely OK, however upper cut levels may be gouging so the tool path is trimmed and reconnected by NCMs:

non-cutting moves

 

8. Go back to the Interpolated Vector dialog and change existing point/ add new ones to increases the margins there:

increased margin

 

Limitations in 7.5.2 are:
  • This method is applicable only for blade finish and not for the rest of operation types.
  • This method is applicable only for cut levels Interpolate from shroud to hub.
  • In any case where the generated tool path is potentially gouging, that segment is trimmed and replaced by NCMs. (Update: starting with NX8 the software automatically attempts to tilt it to avoid the collision)
  • Update: starting with NX8 we support user orientations defined for the upper rail as well.
  • Sometimes as you try to rotate the tool it jumps to a different orientation or rotate against the dynamic handle direction. To avoid that you can press the reset to default when right clicking on the arrow.
  • As a preview option in NX 7.5.2, users should be careful about implementing this in production work.

 

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.

 

Comments
Pioneer
Pioneer

Good morning Mr. Finaro.

 

I am working on a turbo impeller in this days and I have a problem.

 

I am using NX 9.1 with turbomarchinery.

 

The blades are thin and long and the material is aluminium. Finishing the blade after the total roughing of the blades causes strong vibration. The geometry of the blade is simple so I am using Swarf interpolation to have a good cycle time.

I choosed Swarf interpolation and turned off the avoid collision option to stay in contact with the side of the mill (a conical endmill). I tried to finish the blade in many ways but always obtain strong vibration.

 

So now I would try to rough out the blades in 4 steps, and finish any step immediatly after any rough operation.

 

For the roughing I have not problem, but for the finishes, if I turn off the "avoid collision" in the tool axes page, the toolpath works all the blade in 1 pass. Using the 0%-100% options in the levels page doesn't work. I need to turn on the "avoid collision" to obtain what I want, but in this way, the tool don't follow the shape of the blade for all the time, and when I will work the second level, I will obtain a blade with a different shape from the 3d solid and if I turn off the "avoid collision" only in the last level, I will obtain strong vibration on the top of the blade.

 

Suggest?

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