CAM Assist for Mastercam FAQs

There are two main sources for feeds and speeds for CAM Assist-generated toolpaths:

1. They are defined by the user in their TOOLDB file as a Preset.

2. They are calculated by CloudNC Cutting Parameters engine and applied to the toolpath.

In the Tool Use tab of CAM Assist, it is possible to direct CAM Assist to use presets or Cutting Parameter calculations, or a hybrid of both:

Open

Add/edit the tool change time to the Machine section in the Choose file(s) tab of the Cycle Time Estimator:

Open

There can be some ambiguity about the terms “feed per tooth” and “chip thickness”, and whether or not they are the same when tool engagement is less than 50% of the tool diameter. CAM Assist takes the simplest and most literal definitions:

• Feed Per Tooth: the distance that the tool advances per revolution, divided by the number of flutes, ignoring the radial engagement of the tool.

• Chip Thickness: the maximum thickness of radial chips created during fixed engagement roughing toolpaths. Sometimes this is also called the Chip Load.

Sticking with these definitions ensures that the definition of Feed Per Tooth is always the same, whether the toolpath is roughing/finishing, or side milling/end milling. When CAM Assist needs to distinguish between the two (for example in the Cutting Parameters Explorer) the terms as defined above will be followed.

When the RCTF option is enabled, the “FPT” property of the toolpath in Mastercam no longer refers to Feed Per Tooth as defined above, but instead it refers to Chip Thickness, which is why CAM Assist will never enable the RCTF option.

To understand CAM Assist’s approach to “chip thinning”, or “high speed machining”, the two separate sources of cutting data in CAM Assist must be examined:

When feeds and speeds are sourced from the Mastercam Tool Manager database of proven feeds and speeds:

CAM Assist assumes that the Feed Per Tooth is specified according to the above definition, i.e., with chip thinning already taken into account. This is because the Mastercam Tool Manager entries for Cut Parameters do not specify whether the Feed Per Tooth field should be interpreted as a Chip Thickness or not. In order to avoid interpreting the data differently in different circumstances, CAM Assist assumes Feed Per Tooth means Feed Per Tooth always.

If you already have an established database of feeds and speeds specified in terms of Chip Thickness, because you usually enable the RCTF option, then you will need to convert these to Feed Per Tooth so that CAM Assist outputs the toolpath with the correct feed rate. This can be done with a machinist calculator or according to the formula below:

Open

When E>0.5, the Feed Per Tooth and Chip Thickness is the same.

Symbol	Meaning	Example (metric)	Example (inch)

Symbol	Meaning	Example (metric)	Example (inch)
Open	Programmed feed per tooth	0.023 mm	0.0115 inch
Open	The maximum chip thickness	0.020 mm	0.0100 inch
Open	The radial engagement of the cut, measured as mm or inch	5 mm	1/4 inch
Open	The tool diameter	20 mm	1 inch
Open	The radial engagement of the cut as a percentage of tool diameter. When used in the formula above, this should be a number between 0 and 1, not between 0 and 100.	0.25	0.25

When feeds and speeds are sourced from CAM Assist’s Cutting Parameters engine:

Radial chip thinning is always taken into account by the CAM Assist Cutting Parameters engine, and the feed per tooth is increased using the same approach as the RCTF option. Therefore, chip thickness has already been accounted for by CAM Assist and is not required to be accounted for in Mastercam’s dynamic toolpath configuration.