Live Knowledgebase > Spindle motors and tooling > Cutters > Feeds, speeds and direction

Please Wait a Moment
X

Yeti Tool Ltd | Knowledge Base

Search for Answers in our Knowledge Base

Our knowledge base is under maintenance

There may be articles with content missing, if you are after this information please submit a support ticket here.

Feeds, speeds and direction

This article is essential reading to understand how to choose appropriate speeds and feeds for SmartBench.

< Previous | List

Feeds and speeds are some of the most important factors to consider when implementing any CNC strategy.

You enter the feeds and speeds into your tool settings within your CAM software.

What is feed rate?

Feed rate is the speed at which the cutter moves across the face of the material. It is measured in distance units per minute (e.g. millimeters per minute, or inches per minute).

We will refer to this as our movement speed in X/Y.

What is spindle speed?

Spindle speed is the speed at which your cutting tool rotates. It is measured in RPM (revolutions per minute).

Click here to find out more about spindle specifications.

Which direction should I be cutting in?

Feed direction is defined as either climb milling or conventional milling. Each definition simply describes the direction of the feed against the material, relative to the rotation of the cutter. 

You will find this option in your CAM software as you define your toolpath strategies.

Conventional Milling

When the cutter is doing the deepest part of its cut, it is rotating against the direction of the X/Y travel (and is cutting least efficiently).

Note how the width of the chip starts from zero and increases as the cutter finishes slicing.

Climb Milling

When the cutter is doing the deepest part of its cut, it is rotating with the direction of the X/Y travel (and is cutting most efficiently).

Note how the width of the chip starts at maximum and decreases.

Which direction is right for the job?

We would recommend using climb milling on SmartBench whenever possible, because it requires less power to move the cutter through the material.

You may have some scenarios in which you may need to use conventional milling, such as improving accuracy or cutting certain materials.

All of the values in our lookup tables are given using climb milling, so if you need to use conventional milling, then we would recommend reducing your feed rate by around 30% as a starting point.

What feeds and speeds should I start with?

We have put together some recommended nominal feeds and speeds in order to get you started - you will be able to find the quick lookup tables at the end of this article. 

A quick note on Feeds and Speeds Calculators:

Traditionally, you would calculate the feeds and speeds for your CNC machine by measuring chip load and using a formula.

This approach does not work with SmartBench, so you will need to use the lookup tables as your starting point. 

 

Remember, this is just a starting point! There are many factors that can have an impact on your feeds and speeds:

  • Material

  • Cutter (type, material and sharpness)

  • Desired surface finish

  • Desired accuracy

  • CNC machine characteristics

  • Extraction performance

  • Workholding

How do I know if I need to adjust feeds and speeds? 

Before you start a job, you need to know when and how to adjust feeds and speeds. This will help you achieve the perfect finish.

If you are trying something new (e.g. a new material or cutter) you can always cut a test piece first on some scrap material, and try adjusting feeds and speeds throughout the test. 

What to look out for

Blunt cutters

You should always check the condition of your cutter to ensure it is sharp and undamaged. Otherwise you might be trying to get the right feed and speed, when you should actually just change your cutter. 

Click here to learn more about how to check your cutter.

Make chips, not dust

When you are honing your feeds and speeds, always look to make chips, not dust. Chips help to take heat away from the stock material, thus increasing tool life and finished edge quality.

Listen to the tool

Always listen to the sound of the tool as it's cutting. If a router is working too hard you'll hear it, generally as a higher pitched noise.

If you have a Precision Pro model of SmartBench, you may see the spindle overload begin to increase on the console, normally starting at 20%. If it gets beyond that, it’s definitely time to adjust feeds and speeds!

Overheating on the tool or stock material

Signs of overheating give you an indication of tool damage, or incorrect feeds and speeds. This means your cutter is rubbing rather than cutting.

A: Edge without signs of overheating.

B: Edge with signs of overheating.

A: Cutter in original good condition.

B: Cutter has been discoloured due to overheating.

Problem solving

Here is a problem solving map to help you if you start to have issues.

Image credit: CMT Orange tools

How to make adjustments to feeds and speeds mid-job

SmartBench gives you the ability to adjust your feeds and speeds at any time during the job. These can be changed in 5% increments to allow for fine adjustment.

Feeds and speeds: Quick lookup tables

We have tested a range of tools with a variety of common materials. We experimented with different feeds and speeds, and settled on some ballpark starting points.

This data is intended for a new SmartBench user. 

Be aware that there are multiple factors to consider when choosing feeds and speeds. 

The figures shown below are starting points, and you must be able to adjust from these points as required. 

If you skipped the rest of this article to go straight to this section, make sure you go back and read the previous sections, so that you can adjust as needed.

 

Check the quick lookup tables for the following materials:

MDF

YetiTool Part Number

Diameter (mm)

Shank (mm)

Type

Maximum Step Down/Step Over (mm)

Recommended Feed rate (mm/min)

Recommended Spindle Speed (RPM)

20805

3

8

Upcut Spiral

1.5

2,000

18,000

20806

6

8

Upcut spiral

3

2,500

20,000

20807

8

8

Upcut spiral

4

3,000

22,000

20813

3.2

8

Round Nose

1.6

2,000

18,000

20814

6

8

V-Groove

2

2,000

20,000

Plywood

YetiTool Part Number

Diameter (mm)

Shank (mm)

Type

Maximum Step Down/Step Over (mm)

Recommended Feed rate (mm/min)

Recommended Spindle Speed (RPM)

20805

3

8

Upcut Spiral

1.5

3,500

18,000

20806

6

8

Upcut spiral

3

3,000

20,000

20807

8

8

Upcut spiral

4

3,000

22,000

20813

3.2

8

Round Nose

1.6

2,500

18,000

20814

6

8

V-Groove

2

2,500

20,000

Softwood

YetiTool Part Number

Diameter (mm)

Shank (mm)

Type

Maximum Step Down/Step Over (mm)

Recommended Feed rate (mm/min)

Recommended Spindle Speed (RPM)

20805

3

8

Upcut Spiral

1.5

3,500

18,000

20806

6

8

Upcut spiral

3

3,000

20,000

20807

8

8

Upcut spiral

4

3,000

22,000

20813

3.2

8

Round Nose

1.6

2,500

18,000

20814

6

8

V-Groove

2

2,500

20,000

Hardwood

YetiTool Part Number

Diameter (mm)

Shank (mm)

Type

Maximum Step Down/Step Over (mm)

Recommended Feed rate (mm/min)

Recommended Spindle Speed (RPM)

20805

3

8

Upcut Spiral

1.5

300

18,000

20806

6

8

Upcut spiral

3

400

20,000

20807

8

8

Upcut spiral

4

600

22,000

20813

3.2

8

Round Nose

1.6

300

18,000

20814

6

8

V-Groove

2

300

20,000

Plastics

YetiTool Part Number

Diameter (mm)

Shank (mm)

Type

Maximum Step Down/Step Over (mm)

Recommended Feed rate (mm/min)

Recommended Spindle Speed (RPM)

20805

3

8

Upcut Spiral

1.5

2,000

18,000

20806

6

8

Upcut spiral

3

2,500

20,000

20807

8

8

Upcut spiral

4

3,000

22,000

20813

3.2

8

Round Nose

1.6

2,000

18,000

20814

6

8

V-Groove

2

2,000

20,000

Aluminium 6082

YetiTool Part Number

Diameter (mm)

Shank (mm)

Type

Maximum Step Down/Step Over (mm)

Recommended Feed rate (mm/min)

Recommended Spindle Speed (RPM)

20538

6.35

6.35

Upcut Spiral

0.8

460

16,000

Composites

YetiTool Part Number

Diameter (mm)

Shank (mm)

Type

Maximum Step Down/Step Over (mm)

Recommended Feed rate (mm/min)

Recommended Spindle Speed (RPM)

20815

18

8

ACM

2

800

16,000


< Previous | List

If this article didn't solve your problem, please submit a support ticket here

Rami

Rami is the author of this solution

Glad we could be helpful. Thanks for the feedback.

Sorry we couldn't be helpful. Your feedback will help us improve this article.

Did you find it helpful?

Yes   No
Updated on Thu, 08 Jul 2021