PM 05 3doffset+constz
PM 05 3doffset+constz
PM 05 3doffset+constz
Delete All and Reset forms and from File > Examples select the model camera.dgk.
This model is a good example where it is a better option to use more than one finishing strategy. 3D Offset and Constant Z strategies will be used and they will be they will be kept separate by being limited to a Boundary. Before finishing can take place an Area Clearance toolpath will be created to remove the bulk of the material.
Calculate the Block to component size, in Rapid Move Heights apply Reset to Safe Heights, and use Block Centre Safe in tool Start Point. Define a Tipped Radius tool with Diameter 25 and Tip Radius 3 called D25T3. Calculate an Offset Areaclear Model toolpath called RoughOp1 using a Thickness 0.5, Stepover 10 and Stepdown 3. All other parameters can be set to your preference. Simulate the toolpath in Viewmill.
Issue PMILL 6
77
PowerMILL
We are now in a position to define the Boundary. Certain types of Boundary are calculated based on the Active tool. The Tolerance and Thickness values in the Boundary forms are important and normally reflect the same Tolerance and Thickness values with the subsequent toolpaths applied to them.
Right click on the Boundaries icon in the explorer and select Create Boundary -> Shallow.
78
Issue PMILL 6
PowerMILL
Tick the Use Axial Thickness box. Set Radial thickness to 0.5
A Shallow Boundary takes its segments from areas on the model that are defined by an Upper and Lower threshold angle. It is therefore specifically suited to steep walled and shallow surface machining techniques
With Radial Thickness set to 0.5 the stock thickness left on the sidewalls from the roughing will not be machined at this stage.
Make sure that the correct tool is Active, in this case BN10.
Issue PMILL 6
79
PowerMILL
With the model and toolpaths undrawn the Boundary should look something like this. It is made up of numerous segments each one dividing the model into steep and shallow areas. Any of which can be selected and individually deleted at any time (only before being assigned to a toolpath).
Select the Toolpath Strategies icon from the top of the screen. Select a 3D Offset Finishing strategy from the form then OK.
Enter the Name 3D Offset BN10. Select Direction Climb. Enter a Tolerance 0.02. Enter a Thickness 0.
Notice that the newly created, Active Boundary is automatically selected for use. If a different Boundary is required it can be selected from the pull down menu.
Select the Leads and Links icon and set the Lead In to None, Links Short and Long Links to Safe
80
Issue PMILL 6
PowerMILL
The toolpath is calculated following the contours of the Boundary segments and is produced only on the shallow areas of the model. Further improvements can be made to this toolpath with respect to the Links between toolpath tracks. At the moment they are all at Safe Z.
Select the Leads and Links icon from the top of the screen. Select the Links tab and change the Short Links to On Surface, the Long and Safe Links to Skim. Apply and Accept the form.
The toolpath has now is now more efficient with the rapid moves at skim height and the short links being forced onto the surface.
Simulate the 3D Offset toolpath in Viewmill. Right click over toolpath 3D Offset BN10 in the explorer and select Settings from the pull down menu. Select the Copy icon on the form. Rename the toolpath as 3D Offset BN10_Spiral. Tick the box Spiral. Leave all other values the same then Apply and Cancel the form.
Issue PMILL 6
81
PowerMILL
The Spiral option is ideal for HSM (High Speed Machining) applications where ideally toolpaths should be as continuous as possible with the minimum sudden changes direction. Leads and Links are greatly reduced using this method.
Constant Z machining
Constant Z machining projects each tool track horizontally onto the component at fixed heights defined by the Stepdown.
As the component surface becomes shallow the actual tool step over increases until it becomes non-existent on flat areas.
82
Issue PMILL 6
PowerMILL
Enter a Name Constant Z BN10. Set a Stepdown of 1. Enter the Tolerance as 0.02
Set the direction to Climb. Set the Trimming to Keep Outside. Open the Leads and links form and set all the Links to Safe. Apply then Cancel
By using the Boundary Trimming option Keep Outside, the toolpath is correctly limited to the steep areas of the model.
If the Boundary had not been used the toolpath would have looked something like this. It can be seen that the parts of the toolpath on the shallow areas have an excessive Stepover.
Issue PMILL 6
83
PowerMILL
Select the Leads and Links icon at the top of the screen.
Select the Lead In tab and change the 1st Choice to Horizontal Arc Left, Angle 90.0 and Radius 2.0. Click the button Copy to Lead Out.
Select the Links tab and change the Short, Long and Safe to Skim. Apply and Accept the form.
The tool now leads in and out of the toolpath with a horizontal arc. If the tool lifts it will only lift by the skim distance taken from the first page of the Leads and Links form (Z Heights tab). The Rapid moves at skim height are purple in colour while the plunge moves are light blue.
84
Issue PMILL 6
PowerMILL
Closed Offsets if ticked will cause the 3D Offset areas of the machining to be ordered to occur from outside to inside. The reverse applies if Closed Offsets is unticked.
Deactivate the Shallow boundary, BN10_1 in the explorer. Select the Toolpath Strategies icon from the top of the screen. Select an Optimised Constant Z Finishing strategy from the form then OK.
Issue PMILL 6
85
PowerMILL
Enter Name OptConZBN10 Select Closed Offsets Set the Direction to Climb. Input a Stepover value of 1 Make sure no boundary is selected Enter the Tolerance as 0.02
Reset the Lead In and Lead Out to None and set all Links to Safe.
Note the consistent Stepover between tool tracks across the whole component.
Optimized Constant Z has performed well in this example but it does take longer to calculate. Sometimes it is better to use Boundaries with a combination of 3D Offset and Constant Z.
86
Issue PMILL 6
PowerMILL
Select the Leads and Links icon from the top of the screen to bring up the form and select the Links tab. Change the Short links to On Surface. Change the Long and Safe links to Skim. Apply and Accept the form.
Both the Constant Z and 3D Offset parts of the toolpath currently use a 1mm Stepover. By ticking the box Use Separate Offset Stepover it is possible to apply a different, larger Stepover value to the shallow areas created with the 3D Offset strategy used in this hybrid form.
Issue PMILL 6
87
PowerMILL
Introduction to NC Programs.
At this stage we will start looking at post processing a single toolpath from the explorer as an introduction to outputting NC Programs. NC Programs will be covered in more detail later in the course.
All of the toolpaths that have been created in this chapter should appear in the explorer like this. This introduction will concentrate purely on the output of one single toolpath Rough Op1.
Right click over the NC Program (dark green icon) and select Settings.
88
Issue PMILL 6
PowerMILL
The path to where the program will be output. Before post processing can occur the required option file (*.opt) must be selected.
Select the folder icon to open up the Select Machine Option Filename form.
Select the Heid400.opt and then Open. Select Write at the bottom of the NC Program form. Close down the subsequent form, which confirms the output using
The contents of the NC Program can be viewed by double clicking on it in the C:\ NC Programs folder and view it in WordPad.
Issue PMILL 6
89
PowerMILL
Flat Machining
Import the model Flats Create a 20mm diameter End Mill tool named EM20 Calculate the Block and set the Safe heights Open the Offset Flat Finishing form and fill in as below
It should be noted that where a flat is next to a vertical face Flat finishing will finish the vertical as well. Where this is undesirable a Radial thickness should be applied
Accept
90
Issue PMILL 6
PowerMILL
The flat surfaces have been finish machined but material has been left in the area behind the boss and at the bottom of the holes where the 20mm diameter tool could not enter. We will now use a smaller tool to finish these areas.
Create a 10mm diameter End Mill tool named EM10 Copy the toolpath Flat Fin EM20 and fill in the form as below
Issue PMILL 6
91
PowerMILL
The bottoms of the holes and the area behind the boss have now been finished as shown in the Z view below.
92
Issue PMILL 6