Impact User Guide

Engraving Machine Settings

Modified on: Thu, 5 Oct, 2023 at 1:36 PM

The Engraving Machine Settings page can only be configured if the Heidenhain Engraving Machine driver is selected from the General page of the plotter machine, or the Engraving Machine type is selected from the General page of the plotter machine together with either Bosch CC100 Laser, Compumotor WaterJet, General Counter, General Laser, Customer driver, MarbaSet driver or BoxPlan Pinsetter driver.

Machine Attributes - Engraving Settings

General Settings

Plunge feedrate

This is a percentage applied to the actual feedrate when the tool is driven into the material.

Conventional milling

The default direction is clockwise. If this option is unselected, then the path will be created counter-clockwise.

Finished edge first

When milling a shape, the default is to mill from the outside to the inside of the shape. If this option is unchecked then shapes will be milled from the inside to the outside.

Output small arcs as lines

By default small arcs are converted to lines before being output. If this option is unchecked then small arcs will always be output as arcs.

Use tangential entry

The tool will be driven into the material gradually, rather than vertically.

Tangential overlap

This is the horizontal distance that the tool will travel when Use tangential entry is selected.

Conversational mode output

The default output mode is ISO. This option switches to conversational mode.

An example of ISO mode output is given below:-

G0 X-0.446 Y+3.889 Z+50 G40 M
Z+0.5 G40 M
G1 X-0.446 Y+0.889 Z-0.533 F100 M
G3 X+0.446 Y+0.889 X+0 Y+0.889 F500 M

An example of conversational mode output is given below:-

L X-0.446 Y+3.889 Z+50 R0 FMAX M
L Z+0.5 R0 FMAX M
L X-0.446 Y+0.889 Z-0.533 F100 M
CC X+0 Y+0.889
C X+0.446 Y+0.889 DR+ F500 M

Link clearance paths

When an area is being milled out, select this option to join each of the closed paths. This will prevent the tool from being raised and lowered between each path.

Linked clearance path

Unlinked clearance path

Crease channel settings

Number of pecks

Select this option to specify how many passes will be made by the tool to get to the bottom of the crease channel. The size of each peck will be calculated automatically.

For example, the Intermediate drawing for one peck might look like this:-

And the generated code might look like this:-

0 BEGIN PGM ENGSTSP2 MM
1 BLK FORM 0.1 Z X0. Y0. Z-1.
2 BLK FORM 0.2 X+3.786 Y+0.186 Z1.
3 TOOL CALL 1 Z S20000
4 L X+0. Y+0. R0 FMAX
5 L Z+50. R0 FMAX M13 ;Rough tool select
6 L X+23.7 Y+51.907 Z+50 R0 FMAX M
7 L Z+0.5 R0 FMAX M
8 L Z-0.4 R0 F40 M
9 L X+27.3 Y+51.907 Z-0.4 R0 F400 M
10 CC X+27.3 Y+52
11 C X+27.3 Y+52.093 DR+ F200 M
12 L X+23.7 Y+52.093 F400 M
13 CC X+23.7 Y+52
14 C X+23.7 Y+51.907 DR+ F200 M
15 L Z+2.5 R0 FMAX M ;Rough tool off
16 L X+0 Y+0 Z+2.5 R0 FMAX M
17 L Z+50. R0 FMAX M
18 L X+0. Y+0. R0 FMAX M ;Rough tool deselect
19 L M30
20 L M2
21 END PGM ENGSTSP2 MM

But the Intermediate drawing for two pecks might be:-

And the code:-

0 BEGIN PGM ENGSTSP2 MM
1 BLK FORM 0.1 Z X0. Y0. Z-1.
2 BLK FORM 0.2 X+3.893 Y+0.293 Z1.
3 TOOL CALL 1 Z S20000
4 L X+0. Y+0. R0 FMAX
5 L Z+50. R0 FMAX M13 ;Rough tool select
6 L X+23.7 Y+51.854 Z+50 R0 FMAX M
7 L Z+0.5 R0 FMAX M
8 L Z-0.2 R0 F40 M
9 L X+27.3 Y+51.854 Z-0.2 R0 F400 M
10 CC X+27.3 Y+52
11 C X+27.3 Y+52.146 DR+ F200 M
12 L X+23.7 Y+52.146 F400 M
13 CC X+23.7 Y+52
14 C X+23.7 Y+51.854 DR+ F200 M
15 L Z+2.5 R0 FMAX M ;Rough tool off
16 L X+23.7 Y+51.907 Z+2.5 R0 FMAX M
17 L Z+0.5 R0 FMAX M
18 L Z-0.4 R0 F40 M
19 L X+27.3 Y+51.907 Z-0.4 R0 F400 M
20 CC X+27.3 Y+52
21 C X+27.3 Y+52.093 DR+ F200 M
22 L X+23.7 Y+52.093 F400 M
23 CC X+23.7 Y+52
24 C X+23.7 Y+51.907 DR+ F200 M
25 L Z+2.5 R0 FMAX M ;Rough tool off
26 L X+0 Y+0 Z+2.5 R0 FMAX M
27 L Z+50. R0 FMAX M
28 L X+0. Y+0. R0 FMAX M ;Rough tool deselect
29 L M30
30 L M2
31 END PGM ENGSTSP2 MM

Size of peck

Select this option to specify the incremental depth of the tool for each pass. The required number of pecks will be calculated automatically.

Optimise for tool changes

If this option is selected, then all required geometry will be output for one tool before moving on to the next tool. Although this is efficient for tool changes it can add a lot of rapid travel to a job.

The alternative method causes each channel to be milled completely, changing tools as necessary, before moving on to the next channel. This cuts down on rapid travel, and is preferable for machines that can change tools quickly.

Finishing (bottom)

A small amount of material can be left at the bottom of each channel, to be removed by a more accurate Finishing tool. This option specifies the amount to be left.

Finishing (sides)

Similarly, a small amount can be left at the sides of the channel.

Add sloped edges

A chamfer can optionally be added to the top of the channels.

Slope depth

Specify the required depth of the chamfer.

Slope offset

Specify the width of the chamfer.

Tool

Specify from the pulldown list which tool to use for the chamfer. This list will only contain tools that have been specified as Sloping Engraving on the Tool Settings page from the Tool type list.

Add sloped edges