Assignment 1: Drill Jig Plate

First let us look at a sample program for this simple Drill Jig Plate as below:

The program below was created in CIMCO Edit using the NC Assistant macros and general windows editing features. It was refined by testing with the toolpath and later Solid Animation graphics under the Backplot tab in the Editor.

Our goal is to create and test a program in Solid Animation as the one below:

Below you can see a Heidenhain Conversational Dialogue program that will drill the holes and machine the profile contour of the Drill Jig Plate. Each line in the program has a comment associated with it that explains the code. Any lines that do not have an explanation will have been described in a similar earlier block.

It is imperative that the line numbers are sequential and the BEGIN PGM and END PGM have the same program number or name and the same units MM or INCH.

OK, let us look at some Heidenhain Conversational Dialogue code:

0BEGIN PGM 1234 MMProgram Start, 1234 is the program number but could be text
1;MACHINE DRILL JIG PLATEThe semi-colon ; at the start of the line indicates a comment
3;10/05/2021 15:08:09Comment
4;--------------- Comment
5;CENTRE DRILL 11 HOLESOperation comment
6L Z0 R F MAX M91Z axis up to top safe position, M91 invokes machine coordinates programming.
7;CENTRE DRILLTool comment used by Cimco when creating a Tool List
8TOOL CALL 2 Z S800Tool Call to activate the Tool with its offsets and set Spindle speed.
9L X0.0 Y0.0 R F MAX M03Move to position linear at Max Rapid, start spindle forward with M03
10L Z50.0 R F MAX MPosition Z axis
11CYCL DEF 200 DRILLING ~ Drilling Cycle 200
Q200=2.0 ;SET-UP CLEARANCE ~ Drilling Cycle 200
Q201=-2.0 ;DEPTH ~
Q206=35.0 ;FEED RATE FOR PLUNGING ~ Drilling Cycle 200
Q202=-2.0 ;PLUNGING DEPTH ~ Drilling Cycle 200
Q210=0.0 ;DWELL TIME AT TOP ~ Drilling Cycle 200
Q203=0.5 ;SURFACE COORDINATE ~ Drilling Cycle 200
Q204=10.0 ;2ND SET-UP CLEARANCE ~ Drilling Cycle 200
Q211=0.5 ;DWELL TIME AT BOTTOM ~ Drilling Cycle 200
Q395=0 ;DEPTH REFERENCE Drilling Cycle 200
12LBL 1Set Label 1
13L X20.0 Y20.0 R F75 M99Move to hole 1, M99 will execute the Drill Cycle.
14L X40.0 Y20.0 R F M99Move to hole 2, etc
15L X60.0 Y20.0 R F M99
16L X80.0 Y20.0 R F M99
17L X100.0 Y20.0 R F M99
18L X120.0 Y20.0 R F M99
19L X140.0 Y20.0 R F M99
20L X80.0 Y65.0 R F M99
21L X60.0 Y65.0 R F M99
22L X40.0 Y65.0 R F M99
23L X20.0 Y65.0 R F M99Move to hole 11, etc
24LBL 0Set Label End
25L Z50 FMAX M05Move Z axis up from part.
26L Z0 R F MAX M91Z axis up to top safe position, M91 invokes machine coordinates programming.
27M01Option Stop when the switch is set on the CNC control.
28;---------------- Comment divide between operations, optional.
29;DRILL 11 HOLES 8MM DIAHeader comment for drilling similar to Centre Drill.
30L Z0 R F MAX M91
32TOOL CALL 12 Z S4000
33L X0.0 Y0.0 R F MAX M03
34L Z50.0 R F MAX M
Q201=-20.0 ;DEPTH ~
36CALL LBL1Call Label 1 to retrieve the coordinates from Centre Drilling Section.
37L Z50 FMAX M05
38L Z0 R F MAX M91
40;--------------- -
42L Z0 R F MAX M91
44TOOL CALL 5 Z S1800
45L X-25.0 Y42.5 R F MAX M03
46L Z50.0 R F MAX M
47L Z-18 F1500
48L X0 RL F200Start move to contour RL will activate Radius Compensation.
49L Y65
50CC X20.0 Y65.0Absolute Arc Centre.
51C X20.0 Y85.0 DR- REnd point position for X, Y. DR- indicates CW direction.
52L X90
53CC X90.0 Y65.0
54C X110.0 Y65.0 DR- R
56CC X120.0 Y55.0
57C X120.0 Y45.0 DR+ R
58L X140
59CC X140.0 Y35.0
60C X150.0 Y35.0 DR- R
61L Y10
62CC X140.0 Y10.0
63C X140.0 Y0.0 DR- R
64L X20
65CC X20.0 Y20.0
66C X0.0 Y20.0 DR- R
67L Y42.5
68L X-25 R0R0 de-activates Radius compensation.
69L Z50 FMAX
70L Z0 R F MAX M91Z axis up to top safe position, M91 invokes machine coordinates programming.
71M09Stop Coolant
72M05Stop Spindle
73L Z0 R F MAX M91
74M30End of Program M code
75END PGM 1234 MMProgram End, 1234 is the program number but could be text must be the same as the Start.

Now that we've had a look at the program code, we will consider how this was created in the CIMCO Edit. You might want to print the Drill Jig Plate for reference when we are constructing the program.

Let us start by center drilling the holes with a Drill Cycle. We will use Cycle 200 as it has more features than Drilling Cycle 1.

When you have completed entering the hole coordinates test it with the Backplot.

If it doesn’t look like the image above, then debug the entries until it does.

When you have the center drilling working, you can add the 8mm hole drilling by copy/pasting the lines as seen in the image below. We will need to use the hole coordinates again for the drilling so we can use a Label to recall the set of hole coordiantes for the 8mm drilling operations on the holes.

When your entries are correct, you will see the drilling of the deeper holes in the Backplot.

Next we will create the profile starting from a position outside the profile at X-25.0, Y42.2 (1) and moving onto the profile and around in a clockwise direction. The profile will be generated by linear and circular moves using NC-Assistant. The points in the diagram below indicate the sequence of moves.

When you have the profile correct, it will look as in the image below.

The program lines below correspond to the points in the drawing above.

45L X-25.0 Y42.5 R F MAX M03 Point 1, Start Spindle M03
46L Z50.0 R F MAX M Note that the L at the start of the line indicated a linear move
47L Z-18.0 F1500
48L X0 RL F200 Point 2
49L Y65.0 Point 3
50CC X20.0 Y65.0 Arc Centre CC1 – Note CC at the start of the line indicates Circle Centre
51C X20.0 Y85.0 DR- Point 4 – Note C at the start of the line indicates Circular move, DR- Direction CW
52L X90.0 Point 5
53CC X90.0 Y65.0 Arc Centre CC2
54C X110.0 Y65.0 DR- Point 6
55LY55.0 Point 7
56CC X120.0 Y55.0 Arc Centre CC3
57C X120.0 Y45.0 DR+ Point 8, Note DR+ change of Arc direction CCW
58L X140.0 Point 9
59CC X140.0 Y35.0 Arc Centre CC4
60C X150.0 Y35.0 DR- Point 10
61L Y10.0 Point 11
62CC X140.0 Y10.0 Arc Centre CC5
63C X140.0 Y0.0 DR- Point 12
64L X20.0 Point 13
65CC X20.0 Y20.0 Arc Centre CC6
66C X0.0 Y20.0 DR- Point 14
67L Y42.5 Point 15
68L X-25.0 R0 Point 16
69L Z50 FMAX

When we are dealing with arcs at 90 degrees the end points and arc centers are easy to calculate. It's simply a matter of reading the drawing or doing some simple summation. When we are dealing with arcs between lines, that are not at 90 degrees, then we can use a program such as CIMCO CNC-Calc (add-on for CIMCO Edit) to generate the toolpath or do trigonometry calculations as the end points and arc centers are not so easily calculated.

Now that we have created toolpaths to complete the machining and tested their validity, we can complete the program with the other information required to control the Z axis, Spindle, etc. It is an important principle that each tool should be programmed as a small self-contained program so that any tool section in the program can be executed independently if required.

So, each tool section should have a Header, Machining, and End section.

41;MILL PROFILEComment indicating the operation with the Tool in this section (Optional but advisable)
42L Z0 R F MAX M91-Z axis up to top safe position, M91 invokes machine coordinates programming.
43;20MM CARBIDE END MILLTool Description used by CIMCO to create a Tool List (Optional but advisable)
44TOOL CALL 5 Z S1800The Tool and the offset will be activated for Length and Dia. Speed set.
25L Z50 FMAX M05Move Z axis up from part. Stop the Spindle
26L Z0 R F MAX M91Z axis up to top safe position, M91 invokes machine coordinates programming.
27M01Option Stop when switch is set on the CNC control, used when checking is required.

Testing with Solid Animation

When the program is completed, we can test it using Solid Animation to get a better visualization of how the finished part will look. To do this, there’s some setting up to do first.

Before machining, we need to adjust the size to the initial stock using the Solid Setup dialog. By default, Solid Setup will scan the program to get the min/max material sizes. You may, however, want to enter the actual stock sizes to get a better representation.

For this part we recommend the following Solid Setup values:

X Min = -3
X Max = 153
Y Min = -3
X Max = 88
Z Min = -15
Z Max = 0

We suggest selecting the Lock Stock Dimensions while testing the part to stop the automatic scanning. If you want to use the Solid Animation test more than once.

We also need to go to Tool Setup and adjust the tool list to match the tools being used to machine the part.

If we are using Radius Compensation, we must activate this feature.

The final result should look like the image below. The part can be rotated by holding down the left mouse-button and dragging.

A little more programming is needed to clear away the corner before profiling. The programming principles needed to do so have all been demonstrated above.