2L Home

Engraving Tools, End Mills & Cutters
Spring Loaded Engraving Tools
Vacuum Chucks for Workholding

2L inc.

4 Kane Industrial Drive
Hudson, MA 01749
Tel: (978)567-8867
Contact Us
About Us Catalog Contact Us Testimonials Videos Cart

Feeds and Speeds

Feeds and Speeds for Engraving Tools, and Spring Loaded Engraving Tools


Reference the below tables for general Feed and Speed Rates.



TABLE 1 - Feeds & Speeds

Engraving with a Rigid Tool

Tool held in a Collet, End Mill Holder, Shrink Fit Holder, Top Loading Engraving Machines, Other Industrial Engraving or Marking Systems, etc.

Material 3000 RPM 6000 RPM 7500 RPM 10000 RPM  
Aluminum/Aluminum Alloys 6 12 15 20 Feedrates
(IPM)
Brass/Bronze 6 12 15 20
Copper/Copper Alloys 6 12 15 20
Cast Iron, Soft 6 12 15 20
Cast Iron, Hard 2.4 4.8 6 8
Ductile Iron 3 6 7.5 10
Malleable Iron 3 6 7.5 10
Magnesium/Magnesium Alloys 6 12 15 20
Monel/High Nickel Steel 3 6 7.5 10
Nickel Base Hi-Temp. Alloys 2.4 4.8 6 8
Plastics 9 18 22.5 30
Plastics, Glass Filled (i.e. Phenolic) 9 18 22.5 30
Steel, Low Carbon 3 6 7.5 10
Steel, Medium Carbon 4.5 9 11.25 15
Steel, Hardened 1.5 3 3.75 5
Stainless Steel, Soft 3 6 7.5 10
Stainless Steel, Hard 1.5 3 3.75 5
Titanium, Soft 3 6 7.5 10
Titanium, Hard 1.5 3 3.75 5

Copyright © 2015, 2L inc., www.2Linc.com

Please note as with all machining, it is important to take appropriate safety precautions.

RPM= Spindle Speed.
IPM = Inches per minute.
 

Plunge Feed to Depth at 50% of feedrates listed above. Typical engraving depths for permanently marking workpieces are 0.005 0.010.

Notes: To reduce tip breakage on tougher materials or if small tip widths are being used, reduce feedrates above by 50% and make shallow passes (0.001" depth per pass or less is not uncommon on very tough materials). Use of the Tough Tip tool will allow faster feedrates at deeper cuts in tough materials.

Use of the Spring Loaded Engraving Tool will allow significant increase of feedrates and reductions in cycle times. At feedrates above 15 IPM ensure the high speed lookahead feature is enabled on the cnc machine to prevent rounding of corners and sudden starts and stops in corners.

Use of coolant will extend the life of the engraving toolbit.

Engraved lines that appear rough or jagged are usually caused by a dull toolbit or material buildup on the end of the toolbit. Material buildup mostly occurs with gummy materials such as aluminum or copper. Too fast a feedrate or too deep a cut may not allow the material to be cleanly cut. Taking a finishing pass of .001" - .002" deep at a slower feedrate can be used to reduce any burring or jagged edges. Using coolant to engrave helps reduce this buildup. Engraving Cutters are available specifically for softer materials.

Note: Variations in the above table may be required depending on material being engraved and cutting conditions. Consider the above recommendations as a starting point.




TABLE 2 - Feeds & Speeds

Engraving with a Spring Loaded Engraving Tool

Note the Maximum RPM Requirements for each Spring Loaded Engraving Tool Diameter <<< See Below >>>

Material 3000 RPM 6000 RPM 7500 RPM  
Aluminum/Aluminum Alloys 15-25 30-50 37.5-62.5 Feedrates (IPM)
Brass/Bronze 15-25 30-50 37.5-62.5
Copper/Copper Alloys 15-25 30-50 37.5-62.5
Cast Iron, Soft 15 30 37.5
Cast Iron, Hard 10 20 25
Ductile Iron 13 26 32.5
Malleable Iron 13 26 32.5
Magnesium/Magnesium Alloys 20 40 50
Monel/High Nickel Steel 13 26 32.5
Nickel Base Hi-Temp. Alloys 13 26 32.5
Plastics 25 50 62.5
Plastics, Glass Filled
(i.e. Phenolic)
25 50 62.5
Steel, Low Carbon 13 26 32.5
Steel, Medium Carbon 13 26 32.5
Steel, Hardened 10 20 25
Stainless Steel, Soft 13 26 32.5
Stainless Steel, Hard 13 26 32.5
Titanium, Soft 13 26 32.5
Titanium, Hard 10 20 25
Glass & Stone
(with diamond engraving tool - use coolant with spindle rotating or non-rotating)
17 Not Recommended

Copyright © 2015, 2L inc., www.2Linc.com

Please note as with all machining, it is important to take appropriate safety precautions.

RPM= Spindle Speed.
IPM = Inches per minute.

The 3/4" Shaft Standard Spring Loaded Engraving Tool has been tested up to 10,000 RPM and has a 1,000 - 10,000 RPM recommended speed range.

The 20 mm Shaft Standard Spring Loaded Engraving Tool has been tested up to 10,000 RPM and has a 1,000 - 10,000 RPM recommended speed range.

The 1/2" Shaft Mini Spring Loaded Engraving Tool should not be used at speeds above 7,500 RPM and has a 1,000 - 7,500 RPM recommended speed range.

The 3/8" Shaft Mini Spring Loaded Engraving Tool should not be used at speeds above 6,000 RPM and has a 1,000 - 6,000 RPM recommended speed range.

The 1/4" Shaft Mini Spring Loaded Engraving Tool should not be used at speeds above 3,000 RPM and has a 1,000 - 3,000 RPM recommended speed range.

(RPM speeds for the Mini Spring Loaded Engraving Tools are due to the reduced shaft diameter. Bending of the shaft may occur at higher RPMs).
  • Plunge the tool to depth at a rapid feedrate.  For example: G1Z-0.020F350 or G0Z-0.020
     
  • Decrease the feedrate to produce deeper more pronounced marks and increase the feedrate to produce shallower less pronounced marks. 
     
  • When engraving tougher materials, use of the Tough Tip engraving toolbit is recommended. 
     
  • Ensure the high speed look ahead feature is enabled on the cnc machine to prevent rounding of corners due to the high feedrates required.

    It has been observed that when using the latest generation of cnc machines, the fastest feedrate actually obtained when engraving letters 0.200" tall is approximately 80IPM. Increasing the spindle speed beyond 7500RPM requires feedrates that the cnc machines are not capable of providing and provides no additional benefit in cycle time reduction.
     

Use of coolant will extend the life of the engraving toolbit.

Since the Spring Loaded Engraving Toolholder uses a spring to provide the downward pressure against the toolbit, in general, slower feedrates produce deeper more pronounced marks and faster feedrates produce shallower less pronounced marks.

Slow feedrates allow the spring to press the toolbit into the material being marked for a longer period of time and therefore produce a deeper mark. (i.e. if you completely stop feeding the tool, it will just drill down into the material until it is fully extended.)

Fast feedrates cause the toolbit to skim over the material being marked and produce a less pronounced mark. Too fast of a feedrate will cause the tool to skip over the material without cutting it and will produce marks that appear as dotted lines.

A depth controlling nosepiece is available for absolute depth control.

The feeds and speeds listed above are a good place to start and have been used successfully to engrave a wide variety of materials including aluminum, stainless steel, glass, and plastic parts. Increase or decrease the feedrates to achieve the desired results. Note that as you increase your spindle speed, your feed rates increase also. If you do not have a "look-ahead" feature on your machining center or CNC machine, fast feed rates may create a rounding affect on your engraved lettering.

The depth of cut (total amount of spring travel) can be up to .40". For standard engraving on flat surfaces, a depth of approximately Z-0.020 will compensate for normal material irregularities.

Note: Variations in the above table may be required depending on material being engraved and cutting conditions. Consider the above recommendations as a starting point.

 


TABLE 3 - Feeds & Speeds

End Mills

Material SPEED [SFM] D=1/8” D=1/4” D=1/2”
Aluminum/Aluminum Alloys 600-1200 0.0005 0.002 0.004
Brass/Bronze 200-350 0.001 0.002 0.003
Copper/Copper Alloys 450- 850 0.001 0.002 0.002
Cast Iron, Soft 300- 750 0.001 0.002 0.003
Cast Iron, Hard 125- 350 0.0004 0.0008 0.002
Ductile Iron 150- 450 0.0005 0.001 0.002
Malleable Iron 300- 550 0.0005 0.001 0.003
Magnesium/Magnesium Alloys 1100-1600 0.001 0.002 0.004
Monel/High Nickel Steel 225-350 0.0005 0.001 0.002
Nickel Base Hi-Temp. Alloys 50-125 0.0004 0.0008 0.001
Plastics 900-1800 0.0015 0.003 0.006
Plastics, Glass Filled 400-1000 0.0015 0.003 0.004
Steel, Low Carbon 300- 600 0.0005 0.001 0.003
Steel, Medium Carbon 150- 450 0.0006 0.0015 0.002
Steel, Hardened 50- 225 0.0002 0.0005 0.001
Stainless Steel, Soft 250- 500 0.0005 0.001 0.002
Stainless Steel, Hard 75- 275 0.0002 0.0005 0.001
Titanium, Soft 175- 400 0.0005 0.001 0.002
Titanium, Hard 75- 250 0.0003 0.0005 0.001

Copyright © 2015, 2L inc., www.2Linc.com

Please note as with all machining, it is important to take appropriate safety precautions.

RPM = (SFM x 3.82) / D
IPM = (No. of teeth) x IPR x RPM

FOR SLOTTING APPLICATIONS:  Reduce Speed to approximately 80% of the lower values for the particular material being machined.

AXIAL DEPTH OF CUT:  These recommendations are for axial depths of cuts not to exceed 1 times the cutter diameter. On tougher materials, depths per pass as low as 0.001" are not uncommon.

RPM= Spindle Speed.
D = Diameter of tool.
IPR = Inches per rev.
IPM = Inches per minute.
IPT = Inches per tooth.
SFM and SFPM = Surface feet per minute.

 

Note:  Variations in the above table may be required depending on material being machined and cutting conditions. Consider the above recommendations as a starting point.



TABLE 4 - Feeds & Speeds

Armor Mills


Armor Mills are designed for use with rigid cnc machines when cutting or engraving granite or other hard materials.

Control of the depth of cut, the spindle speed, and the cutting feedrate is critical to achieve maximum tool life.

Cutting granite or other extremely hard materials may not be possible with the use of a hand operated tool or the life of the tools may be significantly reduced.

2L inc. has tested the armor mills on granite with a rigid cnc machine and a rigidly held workpiece. 

Feedrates are below:
    Cutting the below piece of granite, 2L used:
Material Recommended Speed (SFPM) and Feedrates (IPT) Cutter Diameter = .078"

Depth of Cut per pass = .020"
Cutter Diameter = .125"

Depth of Cut per pass = .030"
Granite
Stone
Armor Plate
Hardened Steel
50- 125 SFPM

0.0001-0.001 IPT
6000 RPM
F5.0 IPM

Plunge = 2.0 IPM

6000 RPM
F6.0 IPM

Plunge = 2.0 IPM
Broken Taps
and Drills
50- 125 SFPM

0.0001-0.0005 IPT
1500-2500 RPM

Plunge = 0.1 IPM
1500-2500 RPM

Plunge = 0.1 IPM
Copyright © 2015, 2L inc., www.2Linc.com

Please note as with all machining, it is important to take appropriate safety precautions.

Use of coolant is typically recommended  and will extend the life of the engraving toolbit.

The sample of granite shown below was machined at the specific feeds and speeds listed above in the table. The Armor Mills successfully machined for 30 minutes at the above conditions to complete the sample.

Armor Mill and Armor Drill, for milling and drilling hard materials, stone, granite, armorplate, brick, high speed steel, hardened steel.

Note: Consider the above feeds and speeds as a reference point. Variations in the above table may be required depending on material being machined and cutting conditions.

To remove broken taps and drills, it is recommended to feed the tools by hand (handwheel on lowest feedrate) until the tool has plunged far enough into the broken tool to encounter a stable cutting condition.

In other words, as the tool begins cutting into the uneven jagged surface of the broken tool, feed extremely slowly to prevent the tool from walking which will put high side loads on the cutting tool and lead to breakage.

Once the tool is fully into the cut and seems stable, feeding with the cnc control at the above feeds and speeds is possible.

Stones such as granite and marble have different machining properties among different varieties and even at different spots within the same piece of stone.


RPM = (SFPM x 3.82) / D
IPM = (No. of teeth) x IPT x RPM

 

RPM= Spindle Speed.
D = Diameter of tool.
IPR = Inches per rev.
IPM = Inches per minute.
IPT = Inches per tooth.
SFM and SFPM = Surface feet per minute.



TABLE 5 - Feeds & Speeds

Armor Drills

Material Recommended Speed (SFPM) and Feedrates (IPT) Cutter Diameter = .078" Cutter Diameter = .125"
Granite
Stone
50- 125 SFPM

0.0001-0.0005 IPT
1500-2500 RPM
F5.0 IPM

Plunge = 1.5 IPM
1500-2500 RPM
F6.0 IPM

Plunge = 1.5 IPM
Broken Taps and Drills, Armor Plate, Hardened Steel
and Drills
50- 125 SFPM

0.0001-0.0005 IPT
1500-2500 RPM

Plunge = 0.1 IPM
1500-2500 RPM

Plunge = 0.1 IPM
Copyright © 2015, 2L inc., www.2Linc.com

Please note as with all machining, it is important to take appropriate safety precautions.

Note: Consider the above feeds and speeds as a reference point. Variations in the above table may be required depending on the material being machined and cutting conditions.
 

Use of coolant is typically recommended  and will extend the life of the engraving toolbit.

To remove broken taps and drills, it is recommended to feed the tools by hand (hand wheel on lowest feedrate) until the tool has plunged far enough into the broken tool to encounter a stable cutting condition.

In other words, as the tool begins cutting into the uneven jagged surface of the broken tool, feed extremely slowly to prevent the tool from walking which will put high side loads on the cutting tool and lead to breakage.

Once the tool is fully into the cut and seems stable, feeding with the cnc control at the above feeds and speeds is possible.

Stones such as granite and marble have different machining properties among different varieties and even at different spots within the same piece of stone.

RPM= Spindle Speed.
D = Diameter of tool.
IPR = Inches per rev.
IPM = Inches per minute.
IPT = Inches per tooth.
SFM and SFPM = Surface feet per minute.


Shopping Cart
Home Products Tech Help Policies Site Map

Copyright © 2015, 2L inc.