SmartCAM Production Milling Trial: Task 6 ‐ Program the Holes
Task 6
Program the Holes
For this next task, we’ll just hone in on the tasks you need to apply in order to load the steps for this hole machining from the KBM.
Those holes are 10mm, representing an M10 tapped hole. Let’s spot drill them to 11mm diameter, then drill and tap.
There are multiple ways of handling the cutting tools in a SmartCAM program:
Define each tool / step you require ‘on the fly’
Load individual tools / steps from a Knowledge Based Machining library, or KBM for short
Load Groups of tools / steps from a KBM
Load a set of tools / steps you have used in an existing program
Load a set of commonly-used tools / steps, where you have created planner content for each set
Configure SmartCAM to load a set of preferred / default tools / steps when starting a new program
You’ll begin to understand that there is a great deal of flexibility when it comes to tooling, as there is in most things SmartCAM.
We don’t intend to detail all of those methods here. You will be loading additional steps for the hole making task from a KBM.
A sample KBM database is installed as part of SmartCAM. When you become a SmartCAM user you could either modify the content of our
sample or begin a new one and populate it with the Tools and Steps specifically required for your CNC task.
There is much technical information for you to know about the KBM, but that is detail for another time.
Remove the pocket and island profiles from the active group by left-clicking on the Remove All Elements icon
on the Group Select Toolbar.
Remove the Profiling toolpath from the graphics view by right-clicking on any part of it in the graphics view and left-clicking on Mask/Unmask.
Open the Job Operations Planner by left-clicking on the Operations Planner icon on the top toolbar.
You will see the Process Step List, comprising of the steps we have applied so far.
Set the position at which to add new steps:
Left-click on the Step: 20 entry in the Process Step List.
Left-click on the Load Steps… button, which is toward the bottom-right of the Job Operation Planner panel.
The sample KBM is opened.
You could simply and easily add a single step from the KBM. We could have got you to do that three times for the tools we require, but
we’ll go up one notch technically and will show you how to load the three hole tools you require in one go.
Fundamentally, you collect together the tools and / or steps you require from the KBM database; the area across the center of the panel showing
the results of the various filters that you can apply.
You then drop your selection to the area across the lower part of the panel before adding them to the job planner.
It’s a little like that ‘add to basket’ that most of us do online.
First collect a 12mm spot drill.
Left-click in the Op Category field at the top of the panel.
Left-click on Hole Operations
Spot Drilling is the top of the list in the Op Type field. If you like, experiment by Left-clicking in the Op Type field
to take a look at the hole operations. Be sure to ultimately select that Spot Drilling from the list.
Similarly, the Tool Category field should be displaying Hole Tools and the Tool Type should be Spot Drill.
The section at the centre of the panel now contains all of the spot drills defined in our sample KBM.
Left-click on the 12.000 Dia drill, and then use the single down-arrow above the area across the bottom of the panel to add it to your collection.
Now we’ll add an M10 tapping drill and tap.
Our sample KBM database has tapping drills and taps grouped together.
Disable Category/Type by left-clicking on the Category/Type checkbox at the top of the panel.
Left-click in the Groups field, over to the right a little. Left-click the Step Groups option from the drop-down list.
The area below now displays the sets of tool groups that are available the sample KBM database.
Scroll down the list using the vertical slider to the right of that list and left-click on our Feature – Hole Tapped 10.0 entry.
The section at the centre of the panel now displays the drill and the tap we grouped together for an M10 operation.
Left-click on the double down-arrow above the area at the bottom of the panel to add those 2 tools to your collection.
Now left-click on the Accept button at the bottom-right of the panel to add your collection to the Operations Planner.
SmartCAM's flexibility very much applies when creating hole making toolpaths. There are a number of ways to program hole features. For now we are going to focus on one of the simplest -
using a point at the hole center.
You will be creating the 3 points at the hole centres as CAD Layer geometry.
Switch to CAD mode by left-clicking the CAD button at the top-left of the insert properties bar or the CAD text alongside it.
It is convenient to create the center points on the existing Layer 2.
Left-Click on the gray box at the right-side of the Layer: field.
Left-Click the 2:10mm Holes layer in the drop-down list.
You are going to snap to the center of each of those 3 holes.
Make sure that center point snapping is turned on. If not then left-click on it to enable it.
Now create the points.
Left-click on the Create Geometry icon at the top of the vertical toolbar over on the right, and left-click on the Point/Rapid command from the list.
The Point/Rapid command panel is displayed.
Left-click on the Point: field name. The text itself, not within an input field.
You will be creating the point elements using that coordinate mode we discussed earlier.
Place your cursor over the center of one of the holes.
The cursor will change to a cross-hair when you are in the correct position.
Left-click in that position and an XYZ point will be created.
Repeat a centre point snap at the centers of the other two holes.
Now generate hole making toolpath for those 3 point elements.
The active group should not currently contain any elements, but if there are any then remove them from the active group by
left-clicking the Remove All icon on the group select toolbar.
Left-click the Add Elements group select tool from the group select toolbar.
Left-click on each of the 3 point elements you have just created.
The points are now in the active group.
Left-click on the Hole Making icon on the top toolbar and left-click on the Point > Hole command from the list.
Populate the Point > Hole panel with step, hole depth and clearance height settings for each step to apply to the set of points in the active group:
Left-click the gray box to the right of the field labelled 1st and left-click the 30: Spot Drl step
Left-click the gray box to the right of the field labelled 2nd and left-click the 40: Drill step
Left-click the gray box to the right of the field labelled 3rd and left-click the 50: Tap step
Spot Drilling. We said that we would spot drill to a diameter of 11mm.
Left-click within the Type field in the 1st row and left-click Spot Dia from the list
Left-click within the Depth field on the 1st row and type the value 11
Drilling. Those hole elements you created are at Z-20. The bottom of our stock is at Z-25.
Drill through by an extra 5mm at full diameter.
Left-click within the Type field in the 2nd row and left-click Full Depth from the list
Left-click within the Depth field on the 2nd row and type the value 10 (being the difference between the hole and the bottom of stock, plus 5mm)
Tapping. Tap through by an extra 3mm.
Left-click within the Type field in the 3rd row and left-click Full Depth from the list
Left-click within the Depth field on the 3rd row and type the value 8 (being the difference between the hole and the bottom of stock, plus 3mm)
Left-click in the Clear: field and type a value of 3.
Left-click Go and the three sets of hole making toolpaths are created.
Note that there was, in this case, no need to switch to CAM mode to complete that last task. The Point > Hole command switched to each step in turn.
The process will have automatically reversed the direction of machining those holes for each of the three step passes.
Verification:
You may want to unmask the other steps in the toolpath model that we have previously masked, because verifying the holes-only would show rapid
collision moves in material that will be machined by the other steps & processes.
You can then verify your toolpath and generate CNC code. You could try that to experience a collision event
As a reminder, you can get details about Verification by clicking here
Left-click the Utility menu on the top toolbar.
Left-click the Mask/unmask… command on the drop-down menu.
The utility enables you to mask or unmask elements belonging to a specified step or
all steps, Tools, Layers or Work Planes.
If the Steps radio button over on the left is not enabled then left-click on the Step radio button or the text alongside it.
If the Unmask radio button near the center of the panel is not enabled then left-click on the Unmask radio button or the text alongside it.
Left-click on the All button.
Left-click on the Close button to close the panel.
All of the Toolpath you have created is added to the Graphics View.
There are some aspects of programming holes in SmartCAM that we want you to make you aware of.
We used a method to program those holes that was simple to document.
But not quite the simplest to use. When in Step mode, you are able to define a hole at a point
by simply using a Create Geometry > Hole or Group Hole command.
Technically-superior methods are Hole Feature-based. You are able to create a hole feature at a point.
Hole Features have attributes such as through / blind,
taper angle, diameter and more. The hole making toolpath processes associated with hole features are that
little bit more ‘expert’ and automatic than the method we have shown you.
It also occurs to us that if machining large numbers of holes in a component is a requirement in your application, that you’ll likely be thinking What?? I
have to snap to the centre of each hole? A tubeplate, for example, might have hundreds, thousands of holes to machine.
Be assured that there are methods and techniques available in SmartCAM to make it easier and quicker to generate and optimize such hole making toolpaths.
Just that here isn’t the place to cover it. Do speak with us if that is something that you specifically seek.
That completes the toolpath modeling we wanted to cover in this work book.
Well done! Thank you for the time you were able to spend with us!.
There are so many good things that we want you to know about SmartCAM, but they must wait.
But we do want to add a few more remarks that are relevant to the early SmartCAM use you have just experienced.
On-screen origin display. You may have spotted that in a few of our screen captures we did not display an origin and XYZ axis directions.
They were omitted to help make the image just a little clearer for use in this document.
The World Axes and Local work plane Indicator can be turned on and off as a matter of need or preference.
Left-click the Utility menu across the top of the window, then left-click Display Modes.
There are checkboxes to turn on or off the display of the Work Plane Indicator and World XYZ Axes.
Panel Defaults. In most panels you are able to save your options settings by
left-clicking on the File menu across the top of the window and left-clicking Keep Defaults…
Work Planes. We didn’t need to use an origin other than the World XYZ Datum in our example.
There are pre-defined workplanes for the XY, YZ and XZ planes, plus user-defined, named Work Planes
that can used to define either a local datum or an axis rotation.
The latter is not really functionality for Production Milling, however.
If rotary axis positioning is your thing then you need to check out SmartCAM Advanced Milling.
View Filters. A View Filters command is available by right-clicking on either an element in the
List View or in clear space in the Graphics View.
Left-clicking on View Filters… - near the bottom of the list - opens a panel that includes checkboxes to enable or
suppress toolpath, wireframe or surface / solid elements in the views.
Using the view filter in the List View, for example, and suppressing Wireframe and Surfaces results in toolpath-only being listed.
Group Select All Toolpath or All wireframe. Finally, there will be times when you want to group select all toolpath or all wireframe elements.
With the Add Elements for a STEP active group icon on the group select toolbar enabled, a rapid left double-click in the graphics view will add all step elements to the active group.
With the Add Elements for a LAYER active group icon enabled, a rapid left double-click in the graphics view will add all CAD Layer elements to the active group.
