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
On the cutting parameters dialog open the ‘Stock’ tab and key in the blade and hub stocks:
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.
To avoid that you may want to do one or more of the following changes:
“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.
Based on the blank material knowledge set the Tangential Extensions and Radial Extensions to provide full coverage.
Tangential Extension = 50%Tool; Radial Extension = 0% tool
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 Part Axis, Distance = 0
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.
When invoking this dialog you can immediately see the expected cut levels spacing as triangles dynamic preview.
Set the required depth mode:
Set the Range Depth.
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.
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 deg
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.
Maximum Blade Roll Angle = 30 deg
Maximum Blade Roll Angle = 0 deg
Note that reducing this value prevents the tool from leaning towards the blade:
Maximum Blade Roll Angle = 30 deg
Maximum Blade Roll Angle = 0 deg
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 %= 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 Stock ≠ Hub 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).
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.
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.
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.
After generation use the Verify Tool Path 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’.
This way you can navigate between levels using the 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.
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:
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 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.
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.|