What is ShopMill? A real alternative to the DIN/ISO interface
ShopMill is the graphical programming user interface developed for SINUMERIK 840D controls. In Siemens’ own words, ShopMill is a real alternative to the standard DIN/ISO user interface. On a machine equipped with it, ShopMill replaces the classic G-code environment with a working environment of its own.
Calling ShopMill “an easy programming menu” undersells it. It contains a large number of functions aimed at die and mould machining, and those functions noticeably shorten the programmer’s work. One point the source document stresses: ShopMill is no longer limited to programming with standard operation steps — it also supports demanding 3+2 axis and 5-axis applications.
ShopMill or G code? Both live in the same interface
This is the question you hear most on the shop floor, and it is usually framed wrongly. ShopMill and G code are not rivals, because ShopMill contains a powerful G-code programming interface of its own. The source document notes that this interface specifically supports die and mould programs.
In practice the work splits in two:
| What are you doing? | Which route | Why |
|---|---|---|
| Standard 2.5 D work: pockets, slots, holes, spigots, face milling | Operation-step programming | Programmed directly at the machine by entering parameters on screen. No code writing needed. |
| A free-form die program coming out of CAM | G-code editor | A program with hundreds of thousands of G1 blocks is loaded as a file; ShopMill’s G-code side runs it. |
| Speed and tolerance settings for a die program | CYCLE832 inside the G-code editor | The High Speed Settings cycle sits inside ShopMill’s G-code programmer. |
So in a die shop both routes are used on the same day: the pocket in a clamping plate is done with an operation step, the die surface with CAM plus G code.
Setting up the workpiece: the control calculates the offset for you
This is where ShopMill saves the most time. The workpiece setup functions allow the position of the part to be established quickly and accurately. Dedicated workpiece and tool measuring cycles simplify setup, and the offsets are calculated automatically by the control system.
Compared with touching off by hand this changes two things: the measured result is written straight into the zero offset table, and the tool radius calculation is taken out of the operator’s hands.
Measuring a workpiece — which geometries?
The source lists ShopMill’s workpiece measuring cycles for the following geometries:
- Edge — referencing from a single face
- Corner — taking X and Y zero in one operation
- Pocket / hole — finding the centre of an internal feature
- Spigot / rectangle — finding the centre of an external feature
- Plane — establishing the position and inclination of a surface
These measuring functions are reached from the measuring menu in JOG mode. Measuring cycles also let you measure in AUTOMATIC mode, so the program itself can take a measurement and write the result into the offset.
Measuring tools
Tool measuring works the same way and lives in two places: the measuring menu in JOG mode and the measuring menu in AUTOMATIC mode. Tool length and radius are measured and written directly into the tool list.
Tool management and tool life monitoring
ShopMill’s tool management is clearly structured and supports:
- Various tool types
- Tool names as text — calling a tool by name rather than by number
- Replacement tools — switching to a sister tool when the life of one expires
- Tool geometry together with tool lengths, radii and the number of cutting edges
For tool life monitoring three separate criteria can be used: the tool’s workpiece count, its service life (time) or its wear parameters. The point the source makes is this: monitoring is what delivers consistent machining quality — surface finish does not quietly drift off towards the end of a shift.
In a shop running series parts or series dies this is the cheapest way to catch a dimensional drift before the tool breaks.
Operation-step programming: 2.5 D work at the machine
ShopMill’s operation-step programming allows standard 2.5 D operations to be programmed simply and directly at the machine. The source describes it plainly as “an ideal additional feature for die makers”.
The logic is to line up work steps in sequence instead of writing G code line by line: set the work zero → call the tool → mill the pocket → drill the holes → cut the slot. Each step is a screen form; the operator only enters dimensions and cutting values.
Three views side by side
- Program operation steps — the ordered list of work steps
- 2D display — the contour in plan
- 3D display — the part as a solid
When the operator moves onto a step in the list, the corresponding feature is shown on the part. A depth entered wrongly, or a direction picked wrongly, is caught on screen before the machine ever moves.
The G-code editor and CYCLE832 High Speed Settings
The G-code programmer inside the ShopMill interface properly supports die and mould programs. The source makes one point explicitly: the “High Speed Settings” cycle now sits inside the G-code programmer of the ShopMill user interface.
So on a ShopMill machine you do not have to switch back to the standard interface to reach CYCLE832 — the cycle is called from within the program editor.
CYCLE832 asks little of the operator: select the machining type (roughing, pre-finishing, finishing) and enter a tolerance value. All the values in the other parameters have been entered by the machine manufacturer (OEM) and are normally not visible; the OEM can open those fields through password-protected adaptation parameters.
On the programming side the structure the source recommends is clear: ideally, CYCLE832 is written in the main NC program and the subprogram containing the part’s geometry lines is then called. That way the cycle can be applied separately to the roughing and finishing sections.
All of CYCLE832’s parameters — tolerance mode, compressor selection (COMPOF, COMPCAD, COMPCURV), continuous-path mode and G642 corner rounding — are covered in a separate guide.
Simulation: seeing the program before the machine runs it
ShopMill offers a detailed and wide-ranging simulation function for seeing the machined features. The way it works: the control system fully calculates the selected program and displays the result graphically.
One of three display types can be selected:
- Plan view
- Three-plane view
- Volume model (3-D)
Simulation is controlled much like the machine: there are softkeys for start, stop, single-block execution and reset. The simulation speed can be controlled with the Override function — useful for slowing down and watching a critical region.
There are differences by control: simulation is displayed in three planes on the 840D and in a single plane on the 802D sl. Rotating, scaling and zooming are available; the 3D volume model from all views and sections is available on the 840D only.
Quick View: for large die programs
Running a die program of hundreds of thousands of lines through a full simulation takes time. Quick View exists for exactly that reason: it gives a fast display of the tool paths for large die part programs. On this dotted-line screen, all programmed blocks coming from G1 lines are displayed as the resulting axis paths.
What it does not support — worth knowing
Quick View is a feature of the SINUMERIK 840D with PCU 50 and displays only part program lines containing G01 blocks. The source states plainly that the following are not supported:
- Program loops
- Polynomials
- Transformations
G02/G03blocks
Quick View is therefore not a simulation, it is a path preview. It does not replace simulation for collision checking.
Four views and distance measurement
Four views are available: 3-D view, X/Y plane, X/Z plane, Y/Z plane. As you scroll through the program window the position in the graphic changes automatically; two program lines show the block currently marked in the graphic.
The available functions are:
- Searching for a specific block
- Zoom in / zoom out
- Panning and rotating
- Measuring the distance between two points
- Editing the displayed NC part program
Distance measurement earns its keep on the shop floor: as the source puts it, it is very difficult to judge the size of a part from G1 blocks. Select two points and the distance between them is displayed in the field at the bottom of the screen.
External drives: when the die program will not fit in the machine
Die programs not fitting into NC memory is the rule rather than the exception. ShopMill enables direct access to external drives over Ethernet from the Program Manager. Die programs made up of very large numbers of lines can be stored on these drives:
- HMI hard disk (PCU 50)
- Flash card (PCU 20)
- Network drives
- USB memory
Two functions matter when working with an external program. The first is block search: a fast block search can be run in an external program, both with and without calculation. The second is status tracking: in AUTOMATIC mode, selecting Program Overview and then the “External programs” softkey displays the status of the external program on the overview screen as a percentage.
The AUTOMATIC screen also displays machining times — directly usable data for shift planning on long die jobs.
Rotary axis moves in JOG and the engraving cycle
Rotary axes
During workpiece setup, rotary axis movements are carried out easily using all of the swivel softkeys. Entry is made directly or axis by axis, and as the source states, all machine kinematics are supported.
This matters in a die shop running 3+2: when clamping a part with an inclined face you manage the rotary table from the swivel menu rather than positioning it by hand.
The engraving cycle
ShopMill’s engraving cycle supports texts with special characters. Beyond that, the following values can be engraved as text:
- Date
- Time
- Workpiece counter
- Variables
Being able to engrave the workpiece counter straight onto the part removes the need for a separate marking station where traceability is required — a die serial number, a production date.
Points to watch on the shop floor
A ShopMill program does not move to another machine as-is
Operation-step programs depend on the machine’s tool list and kinematics. If you call tools by text name, the program will not run on a target machine that has no tool of that name.
Do not confuse simulation with Quick View
Quick View only draws G1 paths; it does not show loops, transformations or G02/G03 blocks. Collision risk is assessed with simulation.
Do not enter a tolerance smaller than CAM’s
Entering a tolerance into CYCLE832 that is tighter than the one defined in CAM is not appropriate. The contour the control can follow is only as accurate as the contour CAM produced.
Probe calibration is not optional
Because measuring cycles calculate the offset automatically, an error stays silent. A work zero taken with an unverified probe shows up on the first cut.
Do not run series work from a USB stick
External drive support is there for large programs; for continuous production a network drive or the HMI hard disk is safer.
Do not leave tool life monitoring empty
If none of workpiece count, service life or wear parameters is entered, the replacement-tool logic never engages.
Frequently asked questions
Which controls have ShopMill?
The source describes ShopMill as the graphical programming interface for the SINUMERIK 840D, and points to “Operating and Programming ShopMill on SINUMERIK 810D/840D” for the full description of its functions. Whether your machine has ShopMill depends on the choice the machine manufacturer made; the same control can equally be delivered with the standard DIN/ISO interface.
If I use ShopMill, can I still write G code?
Yes. ShopMill contains a powerful G-code programming interface, and that interface exists precisely to support die and mould programs. Operation-step programming and G-code programming are not alternatives to each other — they are two ways of working inside the same interface.
Is ShopMill only for simple work?
No. The source states it explicitly: ShopMill is no longer limited to programming with standard operation steps; it also supports demanding 3+2 axis and 5-axis applications. Operation-step programming itself targets 2.5 D work, but the scope of the interface is wider than that.
Can I call CYCLE832 from inside ShopMill?
Yes. The High Speed Settings cycle sits inside the G-code programmer of the ShopMill user interface and is reached from the program editor. All that is asked of you is to select the machining type (roughing / pre-finishing / finishing) and enter a tolerance; the remaining parameters are set by the machine manufacturer.
What is the difference between Quick View and simulation?
In simulation the control fully calculates the program and shows the result as a plan view, three-plane view or 3D volume model. Quick View simply draws the axis paths coming from G1 blocks quickly, for large die programs; loops, polynomials, transformations and G02/G03 are not supported.
My die program will not fit in machine memory. What now?
From ShopMill’s Program Manager you can access external drives directly over Ethernet: HMI hard disk (PCU 50), flash card (PCU 20), network drives and USB memory. A fast block search with or without calculation can be run in the external program, and the program’s progress is displayed as a percentage on the overview screen in AUTOMATIC mode.
How do I set the work zero in ShopMill?
From the measuring menu in JOG mode you use one of the edge, corner, pocket/hole, spigot/rectangle or plane measuring options. The measuring cycles also work in AUTOMATIC mode. The offsets are calculated automatically by the control system.
What can I base tool life monitoring on?
There are three criteria: the tool’s workpiece count, its service life (time) or its wear parameters. Once these values are entered, ShopMill automatically monitors how long tools have been in use, and with a replacement tool defined, consistent machining quality is maintained.
Sources
- Siemens AG — SINUMERIK Advanced CNC Operation & Programming, edition 05/2010 (SINUMERIK 810D / 840D / 840Di / 802D sl): Section 2.13 Program overview / status of external programs, Section 2.14 Simulating the part program, Section 2.15 Quick View, Section 2.16 ShopMill, Section 2.9 High Speed Settings – CYCLE832
- Siemens AG — Operating and Programming ShopMill on SINUMERIK 810D/840D (the document the source refers to for the complete description of ShopMill functions)