NX3 Launch Demo

High Speed Machining

Demonstration Vignette

Overview:

Introduction

High Speed Machining techniques are critical to the success of machine shops in several industries.
One of the keys to getting the most out of your machine is to program tool motion that is specifically made for high speed cutting.
NX will ensure that you maintain the highest material removal rates without overloading your tool.

Solution (1-4 paragraphs)

NX provides the intelligent, flexible roughing that keeps tools performing their best. Embedding or overloading conditions are prevented, so maximum speed and material removal are achievable.
Semi-finishing to a more consistent remaining stock sets up the finishing passes for success.
A wide variety of finishing patterns is provided to tackle any geometry.
This is a fairly in-depth example of a complete job done with NX, using a wide variety of technology and techniques that are well-suited to high speed machining.

Demo Setup:

Start NX4.
Open part Wheel_Cavity.prt
In the Manufacturing application, bring up the Geometry View of the Operations Navigator and pin it out.
Get familiar with the tool paths and the position to view them in.

Demo Section 1: Show the operations in the NC Setup.

Geometry Objects

We are looking at the Operation Navigator, which shows us all of our operations, as well as other top-level objects that provide information to several operations. We call this approach inheritance.
Double click the Workpiece in the Operation Navigator
Press the Blank button in the selection context row at the top
For example, this Geometry object is called the Workpiece, because it contains information about the target part for machining as well as the blank that represents the initial material
Edit the Blank and show that there are several ways to specify it. Drag the auto-block a bit to enlarge it.
We can provide a solid model to serve as the blank, or we can let the system automatically put an offset around the part to approximate a casting, or we can simply use a block, without actually modeling anything. That is what we have here, and it is easy to make the block the size we like.

OK to close the Workpiece
Edit the MCS by double clicking it.
In the same way, the Machining Coordinate System is information that all of the operations will use, so we specify it here as a parent object. Notice how easy it is to make changes.
Drag the MCS around to place it somewhere convenient.

Roughing

Edit the Rough_All tool path by double clicking it in the Navigator.
Replay the toolpath so we can see it. Leave both the Pause After Display and Refresh Before Display boxes checked, and step through the dozen or so regions to see what the operation is cutting. Don't take a lot of time, but just OK on through the levels.
This first operation roughs out the entire cavity with a fairly large tool. NX makes it easy to address large, complex regions like this.

Click the Cut Levels button and display the cut levels. Use the gestures on the graphics region to change to wireframe viewing and back to solids.
If we take a look at the cutting levels that this operation uses, we see that NX has automatically set them up so that any flat faces within this cavity are addressed by a cut level, so that no extra material remains on top of flat faces. For high speed cutting, it is vital that we are not surprised by unexpected lumps of finish stock.

Edit the Restmill_All toolpath by double clicking it in the Operation Navigator.
Replay the toolpath, making sure that Pause After Display and Refresh Before Display are both selected on the Replay Path dialog.
Click OK about 10 times, to get to the region where the tool is slotting through the material that the larger roughing tool could not reach.
Because large tools cannot rough all the regions of the cavity, we are forced to rough with smaller tools as well. It is important that we cut only the regions not already previously cut. NX is keeping track of this cut material automatically, looking at the previous operations.

Notice that this smaller tool is forced to slot through the material in the outer ring. Slotting motion like this wreaks havok on high speed machining because this overload condition will either break the tool outright or start to damage the coating on the insert. This operation is slotting with a trochoidal motion, looping around so that the tool never suffers an overload condition. NX uses a very flexible and adaptive trochoidal pattern that ensures the roughing tools are not pushed out of their safe operation envelope while roughing out any complex geometry.
Cancel any further Replay display
Edit the Rough_All tool path again.
In fact, lets revisit the first roughing cut and employ this powerful approach here as well.
Change the Cut Pattern to Trochoidal.
Process the tool path
Replay the toolpath, making sure that Pause After Display and Refresh Before Display are both selected on the Replay Path dialog.
Click OK about 10 times to get to a level where the pattern is going around the bosses and showing trochoidal motion in the tight turns of the pattern

Islands and strange geometry are no problem for the trochoidal pattern. Notice how the loops get smaller as needed to work into tight corners or negotiate narrow slots. This kind of pattern flexibility is essential to achieving high efficiency cutting, no matter what kind of geometry is encountered. By keeping the tool out of overload conditions, the speed and stepover can be set to maximize material removal without fear of damage.
Now that the first operation has been changed, NX knows that the second roughing operation depends on its results to know where the uncut material is. The red circle shows that the second rough operation needs to be re-processed.
Right-click the Restmill_All operation in the Navigator, slide down the RMB menu to Generate
Now all or our roughing is up to date, and taking advantage of these powerful high speed patterns.

Z_Level

Edit the Z_Level_Outer_Rim operation
Generate the tool path.
We'll go ahead and generate the toolpath on this operation. Now we are finishing (or semi-finishing) our die, so we use techniques that are best for high speed machining. High speed controls work very well with Z-level toolpath. They do a very good job of maintaining speed and handling acceleration and deceleration through corners with look-ahead and advanced interpolation algorithms. So we use Z-level as much as possible for high speed finishing.
Pick the Part button in the geometry selection context row at the top
Select Display to show the selected face
Notice that we simply have to select a face to apply toolpath to the region of interest. Other software (delcam) requires much more use of trimming boundaries or other ways to limit toolpath. In NX is it as simple as it gets: pick a face, machine a face.
Zoom in on the ramping step-downs

As good as Z-level cuts are for high speed machining, it is better yet if the tool can just keep cutting continuously all the way down this face. Notice that the step-downs for this toolpath are continuous shallow ramps from one level to the next. This provides the continuous cutting we want with the Z-level cut style that works so well on high speed controls.
Small details can make a difference in how effectively we maintain our high speed cutting as well. Here is an example where user control is important to getting the best results. The starting point for this cut is tucked into the narrow part of the ring, but we'd prefer it to approach in a more open area. A quick change to the start point will address that.
Click the Points button to access the Control Geometry dialog
Click the Edit button for Cut Region Start Points to access the Cut Region Start Points dialog.
Click the Remove radio button and select the visible start point in the graphics region
Click the Append radio button and the Generic Point button to access the Point Constructor dialog.
Choose the Point on Surface option and select the top face of the cavity near where the new engage point should be. Select a spot that is between the obstacles. The new engage points will be positioned close to the point you pick.

OK, OK, OK, Generate, to see the results of the change
Notice how fast that processed? Again, NX is intelligent about re-calculating. Only the engages changed, so that is all that was re-calculated. This result is much nicer.
Edit the Z_Level_Posts operation by double clicking it in the Operation Navigator, as before
Click OK on the Information dialog.
This operation has been performed once, then rotated around to each of the posts. This message reminds us that any changes made here will be reflected in those other locations as well -- perfect!
Replay the tool path.
Zoom in on the ramping step-downs, as before

Here we are finishing the posts, using the same Z-level cut style with the continuous ramp-down cutting. Again, NX is automatically making sure that a cut is taken at any level with a horizontal face -- we don't want to leave any stock behind on such a face.
Select the Cut Levels button to access the Cut Levels dialog
Change the view to Static Wireframe, using the tool bar at the top
Show the cut levels, using the flashlight button at the bottom of the dialog
Select the Downward arrow to make the second range level current.
In this case, however, we have not yet finished the floor, so I don't want the tool to go quite that far down the post -- that would cause extra embedding and overload the tool.
We can see here that the bottom depth is a bit above the floor. We accomplish this with a simple adjustment of that lowest depth
Grab the vertical slider bar with the mouse and drag it up a bit more than would be reasonable, so it is easy to see the difference.
We'll move it some more, so it is easy to see the change.
OK the Cut Levels dialog
Process the operation.
OK the Z_Level_Profile dialog

Notice that all four posts have a new set of tool paths that stop significantly short of the floor. That was really more than we needed, so...
UNDO
Undo takes us right back.

Area Milling

Edit the Contour_Center operation
Replay the tool path
Zoom up to see the results

This is a simple Area Milling approach that is typical for more-or-less horizontal areas. Notice how the stepover handles the steep area of this center depression though.
Use the Wrench icon to edit the Drive Method parameters
This is a result of specifying the stepover to be done on the part, rather than simply projected from a plane. Again, we are making sure that our high speed cut does not encounter more material than it should. In roughing, this is an obvious concern, but it matters for finishing too (-- remember that's why we stopped just short of the bottom when we finished the posts)
Change from the radio button for stepover applied On_Part to On_Plane
OK
Process
We can compare the results of a simple projection, and see that we'll be digging into more material than we want as we get down to the bottom of this depression.
OK
Zoom in on tool path
That's not what we want. Let's, just...
UNDO
Undo that and get back the better result we had with the On-Part stepover.
Edit Z_Level_Profile operation
Replay tool path

Again, we want to do as much with Z-level cutting as we can, so we are finishing the remaining parts that are not too flat with a Z-level cut.
Edit Contour_Spoke operation
Replay the tool path
The flatter areas we'll finish off with more area milling techniques.
Click the Wrench icon to access the Area Milling Method dialog.
Click the Pattern pull down arrow to show the available cutting patterns.
Hover the mouse over the last pattern, Concentric Arcs.
There are lots of patterns to choose from, but a notable one is to use Concentric Arcs to define the strokes. In this wheel die, that is an ideal choice.

Let's try a different one just to see.
Change the pattern to be Parallel Lines
OK
Process tool path
Again, there are lots of choices, which is important because dies and molds come in an infinite variety of geometries. NX has all the patterns you could want to address whatever geometry comes your way.
Of course, we liked the arcs better in this case, so...
UNDO
Let's go back to that result.

Flowcut

Edit the Flowcut_Spoke operation
Replay the tool path.
Zoom in on the area to see the valleys selected

Click the Dependencies bar at the bottom of the Operation Navigator to display the Dependencies section.
Select the Contour_Spoke operation in the Navigator and point out the Ball_6 tool used in that operation.
Click the icon next to the Reference Tool Diameter value (looks like a lock) and show that the value can be inherited from previous ops or set by the user.
The reference tool diameter tells the software how much material is left uncut. It can be inherited from the previous operations or set by the user. In this case, we want to ensure a bit of overlap between this operation and the one that finished these faces, so we have specified a reference tool a bit larger than the actual tool.
Select the More tab on the Flowcut_Ref_Tool dialog.
These valleys have been automatically detected according to the Flowcut parameters as seen here. There are options for concavity, and minimum length, which filter out unwanted little spurs. But still, sometimes a user wants to control a bit more closely which valleys are being cut. This is done easily with the Manual Assembly feature.
Select the Manual Assembly check box

Process the Operation
Now when the operation is processed, the user has a chance to work on the identified valleys before the tool path is completed. Each branch of the operation is listed, and the user can manipulate each one as he chooses.
Select the different regions in the list and show the corresponding branches of operation in the graphics window
Direction can be changed, the order of cutting can be changed, branches can be split, or smoothed. In this case, we might want to skip the side branch and concentrate only on the U-shaped valley around this region.

Select the FlowCut1 branch and hit the Cut button to remove it from the list.
In this case, we will simply remove the side branch from the operation and continue.
OK

You can see how easy it is to work with the different valley branches to get precisely the finish cutting you want in NX.

Last Details

Zoom out far enough to see all for bosses, plus a bit.
Edit the Contour_Around_Posts operation.
The last operations are taking advantage of a couple more of NX's finishing approaches.
Replay the tool path.

This is a straightforward Area Milling drive method that is very well suited to relatively flat areas. Notice the nice collapse of the offset pattern away from all of the part faces. Some other softwares (Delcam) collapse a pattern like this from only the outer boundary, which would make for some questionable results up against these bosses, in this case.
Zoom out far enough to see the entire cavity.
Edit the Contour_Rim operation
Replay the tool path.
Zoom in to see the tool path

This last tool path is another Concentric Arc pattern, and finishes up the floor of this outer ring. And with that, this cavity is complete.
This last operation finishes the floor of the outer groove, and is another example of cutting with a concentric_Arc pattern. And with that, this die is finished.

Summary

From top to bottom, this NC Job demonstrates the attention to detail that makes NX Machining so effective for High Speed Machining:
Roughing operations that never overload the tool, and automatically keep track of previously cut material
Z-Level finishing operations that provide the high-speed advantages of waterline finishing with the never-stop efficiency of spiral cutting.
Automatic depth control that makes it easy to adjust for cutting preferences (we saw the way we could take that last depth up off the floor a bit when we finished the bosses ... easy!!)
On-Part stepovers make it easy to work in areas that change from steep to not-so-steep without struggling with scallop (or cusp) heights.
Automatic valley cutting for the finishing touches reserves the smallest tools for only the regions that require them. The power of automatic selection with the control of user preference makes this a very powerful way to finish out the last valleys.
Thank you.