Siemens SINUMERIK 828D Function Manual page 159

No intermediate rounding blocks
An intermediate rounding block is not inserted in the following cases:
• The axis stops between the two blocks.
This occurs when:
- The following block contains an auxiliary function output before the movement.
- The following block does not contain a path movement.
- An axis is traversed for the first time as a path axis for the following block when it was previously a
positioning axis.
- An axis is traversed for the first time as a positioning axis for the following block when it was previously a
path axis.
- The previous block traverses geometry axes and the following block does not.
- The following block traverses geometry axes and the previous block does not.
- Before tapping, the following block uses G33 as preparatory function and the previous block does not.
- A change is made between BRISK and SOFT.
- Axes involved in the transformation are not completely assigned to the path motion (e.g. for oscillation,
positioning axes).
• The rounding block would slow down the part program execution.
This occurs:
- between two very short blocks.
Since each block requires at least one interpolation cycle, the added intermediate block would double the
machining time.
- If a block transition with G64 (continuous-path mode without rounding) can be traversed without a
reduction in velocity.
Corner rounding would increase the machining time. This means that the value of the permitted overload
factor (MD32310 $MA_MAX_ACCEL_OVL_FACTOR) affects whether a block transition is rounded or not.
The overload factor is only taken into account for rounding with G641 / G642. The overload factor has no
effect in the case of rounding with G643 (this behavior can also be set for G641 and G642 by setting
MD20490 $MC_IGNORE_OVL_FACTOR_FOR_ADIS = TRUE).
• Rounding is not parameterized.
This occurs when:
- in the case of G641 ADISPOS= 0 in G0 blocks (default!).
- In the case of G641 ADIS = 0 in non-G0 blocks (default!).
- For transition from G0 to non-G0 or non-G0 to G0, the smaller of the values for ADISPOS and ADIS will
apply in the case of G641.
- For G642/G643, all axis-specific tolerances are zero.
Basic Functions
Function Manual, 09/2011, 6FC5397-0BP40-2BA0
B1: Continuous­path Mode, Exact Stop, LookAhead
3.3 Continuous-path mode
159