Configuring TNC 407 Radius Allowance with Q Parameters

The command path starts with the programmed tool call, passes through the active tool-data source, applies any accepted delta, and reaches cutter compensation as an effective radius. Follow that path in order. Writing a value into the status parameter Q108 does not replace the radius source.

Where does the TNC 407 get the compensated radius?

The contour block does not calculate its own tool radius. Cutter compensation uses the tool data active at the time the contour is executed. The relevant path is:

1. The program selects a tool with TOOL CALL.
2. The control obtains the tool length and radius from the active tool-data source.
3. If the installed control accepts DL and DR, it adds those deltas to the called tool data.
4. The control publishes the resulting active radius through Q108.
5. The compensated contour uses that effective radius.

Item	Role	Can it command a new radius?
TOOL CALL	Activates the selected tool and its applicable data	Yes, through an accepted DR entry or changed source data
Active tool table	Supplies the stored tool radius	Yes
TOOL DEF	Defines tool data, but has limited effect when a tool table is active	Not for overriding an active table at the following call
Q108	Reports the currently effective radius	No; treat it as a query value

Call the tool and display or evaluate Q108. Confirm that it matches the currently active radius before changing any contour logic.

Which TNC 407 input fields are actually available?

Check the installed control at the keyboard instead of deciding from the family name. Reported TNC 407 configurations differ: one accepted only the tool number, spindle axis, and speed in a call such as TOOL CALL 1 Z S2000, while a TNC 407A with a 286 processor exposed the length and radius allowance fields. The presence of a FORMULA softkey also differed.

Observed interface	Available path	Next action
DL and DR appear after the basic call fields	Program the allowance in TOOL CALL	Use DR+0,2 for roughing and DR+0 for finishing
The call ends after tool, axis, and spindle speed	No direct delta field is exposed in that editor	Use a Q parameter as the radius entry in the tool table
A FORMULA softkey is absent	Formula entry may not be available in that installation	Do not change an unidentified machine parameter; use the available tool-data path

Enter or edit a TOOL CALL, press ENT through all prompts, and revisit the completed block with the arrow keys. Confirm whether DL and DR can be selected before choosing the programming method.

Why does changing Q108 fail to change the contour?

Q108 carries the current effective tool-radius value toward the program as status data. It is not the upstream radius input consumed by cutter compensation. A calculation that targets Q108 therefore does not provide a dependable way to alter the called tool geometry.

The proposed arithmetic also contained a separate syntax problem. Subtraction must identify both the destination and the source:

FN2: Q108=Q108-0,2

Correcting that expression does not change the parameter's role. The required correction is to move the adjustment upstream: either enter DR in the tool call or change the Q parameter referenced by the tool-table radius.

Expression or setting	What it does	Use for roughing allowance?
Q108	Reads the active radius	No
FN2: Q108=Q108-0,2	Complete subtraction syntax, but aimed at a query parameter	No
DR+0,2	Adds 0.2 to the effective radius	Yes, when the call exposes DR
Q parameter in the tool-table radius field	Makes the stored radius program-selectable	Yes, when direct DR entry is unavailable

Change the selected upstream input, call the tool again, and read Q108. The check passes only when the reported active radius changes by the requested amount.

How do DL and DR alter the compensation result?

DR is the delta radius. A positive value makes the control calculate the cutter as larger. With compensated milling, that moves the tool center farther from the programmed contour and leaves more material. The supplied roughing example uses DR+0,2, which leaves a 0.2 mm radial allowance; DR+0 removes that programmed allowance for finishing.

DL is the delta length. A positive value makes the calculated tool longer, so the controlled point remains farther from the workpiece along the active tool axis. Do not use DL to create a radial contour allowance.

Setting	Calculated tool	Geometric effect
DR+0,2	Radius larger by 0.2 mm	Leaves 0.2 mm on the compensated contour
DR+0	No programmed radius delta	Uses the underlying tool radius for finishing
DL positive	Tool calculated as longer	Moves the tool point farther from the workpiece axially

Run a controlled test move away from the part and compare the indicated effective radius for DR+0,2 and DR+0. Confirm a 0.2 mm difference before executing the contour.

How is DR entered when the call supports allowances?

Complete every prompt in the tool-call editor. After the tool number, spindle axis, spindle speed, and any other displayed fields, continue with ENT until DL and then DR appear. If the block was already completed with END, select it again and use the arrow keys to reach the allowance fields.

1. Call the roughing tool and enter DR+0,2.
2. Execute the contour label once.
3. Retract to a clearance position suitable for the machine and setup.
4. Call the same tool again with DR+0.
5. Execute the same contour label for the finishing pass.

TOOL CALL 10 DR+0,2
LBL CALL 1

TOOL CALL 10 DR+0
LBL CALL 1

The fragment shows the radius states, not a complete machining program. Retain the required spindle axis, speed, feed, approach, retraction, and machine functions from the validated job.

Inspect both completed TOOL CALL blocks. Confirm that the first contains DR+0,2, the second contains DR+0, and the same contour label follows each call.

How is the radius changed when DR is unavailable?

Place a Q parameter in the tool table's radius field, then define that parameter before calling the tool. The documented example assigns tool 66 a radius entry of Q66 in the tool table:

Q66=5
TOOL CALL 66

That call makes the control calculate tool 66 with radius 5. For a two-pass contour, assign the roughing radius before the first call and the finishing radius before the second call. If the underlying finish radius is 5.2 mm and the required radial stock is 0.2 mm, the derived roughing radius is 5.4 mm:

Pass	Radius value	Calculation
Roughing	5.4 mm	5.2 mm + 0.2 mm
Finishing	5.2 mm	Underlying finish radius

This numerical case assumes that 5.2 mm is the validated finish-compensation radius for the called tool. If the shop uses a different measured or corrected value, calculate both pass values from that value rather than from the nominal cutter diameter.

1. Edit the intended tool-table row and replace its fixed radius with the chosen Q parameter.
2. Assign the roughing effective radius to that parameter.
3. Execute TOOL CALL so the new value becomes active.
4. Run the contour label.
5. Assign the finishing radius to the same parameter.
6. Execute TOOL CALL again before repeating the contour.

After each call, compare Q108 with the Q value assigned to the radius field. Confirm the roughing and finishing values independently.

Why does TOOL DEF not override an active tool table?

When a tool table is present and active, the following TOOL CALL uses and calculates with the value stored in that table. A preceding TOOL DEF does not override the table's radius for that call; in this configuration, it serves to prepare the changer for the next tool change.

For that reason, this proposed path does not solve the radius problem with an active table:

FN1: Q10=Q108+0,2
TOOL DEF 1 L=Q114 R=Q10
TOOL CALL 1 Z S2000

The arithmetic places the desired value in Q10, but the subsequent call reloads the selected tool's radius from the active table. The value assigned through TOOL DEF loses the precedence decision.

Configuration	Radius source used at call	Programming decision
Active tool table with fixed radius	Fixed table value	Use DR if exposed
Active tool table with Q parameter in radius field	Current value of that Q parameter	Assign the Q value before each call
TOOL DEF immediately before a call using an active table	Active table value	Do not use this as a radius override

Change one candidate source at a time, call the tool, and observe Q108. Confirm that table edits or DR affect the active value while the preceding TOOL DEF does not.

How should the repeated contour be organized?

Keep the contour in one label so both passes execute identical geometry. Place each radius-state change and tool call outside the label. This prevents the label from silently reloading the wrong state and avoids duplicating the contour blocks on a control with limited editing functions.

Set roughing radius state
TOOL CALL
LBL CALL 1

Retract and stop as required

Set finishing radius state
TOOL CALL
LBL CALL 1

LBL SET 1
Contour blocks
LBL SET 0

Do not merely reset a Q parameter after the first label and enter the second label without another tool call. The tool call is the activation boundary: it causes the control to read the tool data and form the effective radius used by compensation.

If a Q parameter supplies the table radius, initialize it explicitly before the first call. Reset it to the finish value before the second call rather than relying on a prior program's retained state.

Step through the control flow without cutting. Confirm the sequence is roughing value, first tool call, first label execution, finishing value, second tool call, and second label execution.

How is the complete radius path verified?

Verify each hop before allowing the cutter to enter material. Layer one first: confirm the intended tool is installed, its table row is the row selected by TOOL CALL, and the table radius field contains either the validated fixed radius or the intended Q reference.

1. Open the roughing call and confirm whether the selected method is DR+0,2 or a Q-backed tool-table radius.
2. Execute the roughing tool call in a controlled mode and read Q108.
3. Record that effective radius as the roughing state.
4. Apply DR+0 or assign the validated finishing radius to the table's Q parameter.
5. Execute the finishing tool call and read Q108 again.
6. Confirm that the finishing effective radius is 0.2 mm smaller than the roughing effective radius for the stated 0.2 mm allowance.
7. Run the contour in single-block or an equivalent controlled proving mode with the tool clear of the workpiece.
8. Confirm that both passes call the same contour label and that the radius state changes only at the intended tool calls.
9. Machine a controlled test and measure the remaining roughing stock before authorizing the finish pass.

The path passes only when the programmed source, called tool data, Q108 value, compensated motion, and measured stock all agree.

FAQ