CAM WORKFLOWCoordinate systems, post, DNC

⌖How to define the work coordinate system (program origin)

• An NC control has a machine-specific “machine coordinate system” and a “work coordinate system” placed to fit the part. Register where the work origin lies in the machine coordinate system in a work coordinate system offset (G54, etc.).^[1][2]
• The CAM WCS (work coordinate system) is the coordinate reference in which the post-processed NC program is output. The origin is chosen from the model origin, a selected point, a corner of the stock box, a corner of the model box, and so on.One source / reference^[3]
• Point the Z axis away from the surface being cut (toward the tool).One source / reference^[3]
• On the machine, pick up the part's position with an edge finder or touch probe, and register the same point as the origin set in CAM into the work coordinate system.One source / reference^[2]
• Tip:Place the CAM origin at a point that is easy to pick up on the machine (a stock corner, the top surface, a hole center, etc.).One source / reference^[3][2]

G-code dictionary:G54–G59,G92,G53,G43 (tool length compensation)

▦Defining the stock

• In a CAM job (setup), enter the size and shape of the stock that machining starts from. Entering the stock reduces air cutting.^[4][5]
• A function that tracks the stock remaining as operations proceed (in-process stock update) can be used for rest machining, reducing air cuts, and checking for collisions.^[5][6][7]

⊓Tool library

• A register of tools (shape, diameter, flute length) and holders. Each CAM has its own tool library or tool table.^[4][8][6]
• Some machines' tool offset tables also hold the number of flutes, material, and so on, in addition to tool length (H) and tool diameter (D), and use them for guideline calculations of feed and speed.One source / reference^[2]

For holder, collet, and spindle taper dimensions, seeToolingpage.

÷How to enter cutting conditions

• Enter speed, feed, and depth of cut for each tool. The idea in high-efficiency roughing is to keep the radial engagement small and take a deep axial depth of cut instead.^[9][10]
• In some software, CAM's internal feed unit differs from the NC program's unit (mm/min, etc.). When entering conditions by hand, check the unit field.One source / reference^[4]

The guides for trochoidal slot milling and for the first depth of cut in high-efficiency roughing can be calculated on theToolpath types page. For speed and feed, see theEnd mill and milling cutter calculator.

◎Simulation and collision check

• Toolpath and cutting simulation in CAM:Plays back the path inside CAM and shows how the stock is cut away and where the tool makes contact. Done before the post.^[11][12][4]
• Machine simulation:Shows even the machine structure (table, spindle head, rotary axes) on screen to check collisions among tool, holder, fixture, and machine, and stroke overruns. Especially needed for 5-axis and multitasking machining.^{[6][13][14][15]}
• NC program verification (after post):Loads the NC program produced by the post itself and reproduces the machine's motion to check it. It does not depend on CAM. Typical examples are VERICUT (CGTech, USA) and NCVIEW (Simpletech, Japan). NCVIEW also simulates macro programs and estimates machining time.^[16][15]
• NC control graphic display:Without moving the machine, have the NC control's screen draw the path to check it. Some controls color-code rapid and cutting feed.One source / reference^[17]
• CAM-TOOL has an integration function with VERICUT (C&G Systems product page)^[18]

For collision checking on 5-axis machines, see5-axis calibration, collision, fixtures and tools.

⇢Post-processor

• Role:Software that translates the machine-independent path data (CL data) that CAM creates into an NC program for a specific machine and NC control. It absorbs differences in the machine's axis configuration, available G/M codes, and format.^[19][4]
• Why it matters:Even for the same path, you do not get a correct NC program unless the post suits the machine. A distributed generic post does not necessarily suit your machine either, so test a new post carefully.^[20][4]

How to choose and fix one

• First choose a generic post that suits your machine and NC control. A distributed post does not necessarily suit your machine as is, so try a new post with care.^[20][4]
• If nothing fits, rewrite or create a post. The post language and authoring tool differ by CAM (Fusion uses JavaScript, FreeCAD uses Python, NX uses Post Configurator, Creo uses GPOST).^{[20][4][22][8]}
• Verify a post you made by cutting a complex curved surface on the actual machine.One source / reference^[19]
• Output settings such as the unit (G20/G21) are determined by the post or the job's output settings. Saving them in a template prevents forgetting the setting each time.One source / reference^[4]

How posts are provided (by software)

For how to read the NC program that comes out, seeG/M code dictionary.

⇄DNC operation and memory operation

• The NC control's capacity for storing NC programs is limited, and a large program cannot be run from the control's memory. Many NC controls have communication functions and support DNC operation (remote buffer operation), which machines while the program is fed from an external source.One source / reference^[24]
• When connecting by RS-232C, match the I/O channel, baud rate, stop bits, and so on in the NC control's parameters. The details of the settings differ by equipment maker and age.One source / reference^[24]
• Communication cables come as a 3-wire crossover without flow control and a handshake-type crossover. Pin assignments differ by equipment and number of terminals, and a mismatch causes communication failure.One source / reference^[24]
• Handing the plan made in CAM to the factory through a connection to the shop floor linked with DNC and PLM is the CAM workflow in the broad sense.One source / reference^[25]
• Case study:Kumamoto University case: DNC operation over RS-232C on a Makino KE55 (FANUC Series 20i-FA, 9,600 bps). NC data for a propeller, created in CAM by raster machining, was split into files of 200 KB or less (cycle time within 5 hours) and run.One source / reference^[24]

!Common mistakes (before the first run)

Checking an item only marks it; nothing is saved anywhere.

• Mixed-up coordinate systems:The origin set in CAM does not match the work coordinate system (G54, etc.) registered on the machine. One of the main causes of first-run collisions. How to prevent: on the first run, check the path with the NC control's graphic display, and use safe-operation functions if available.^[17][3][1]
• Tool length setting mistake:If the tool offset (tool length H) value is wrong, or the number called is wrong, Z goes off and the tool collides. Tool offset errors are a frequent cause of first-run collisions.^[17][2][1]
• Wrong tool in the spindle:The tool number in the program differs from the actual tool. Along with tool offsets and work coordinates, a cause of collisions.One source / reference^[17]
• Collision during rapid moves:Most CAM operations do not know about clamps or fixtures, so rapid-move paths can hit the fixture. Include the fixture in the model and check it by simulation. Some machines have a first-run function that detects a collision during rapid moves early and stops (it does not detect during cutting feed).^[4][17]
• Mixed-up units:Mm and inch get mixed up when reading data without units such as STL, or through differences between CAM's internal unit and the post's output unit.^[26][4]
• Post that does not fit the machine:Outputting with a generic post as is can produce codes for functions the machine does not have, or a different format. Try new posts carefully.^[20][4]
• Missing faces in received data:When STEP or IGES is imported, faces fail to join and the path gets created on a model with holes in it. After importing, stitch the faces and run a shape check.^[27][4]

Related commands: tool length setting mistake →G43,G49　mixed-up units →G20,G21

Printed from Kezuriba (kezuriba.net/en/cadcam/workflow/)