Commit 8c8352cd by Grace Copplestone

### copied from fab server

parents
calculator.html 0 → 100755
This diff is collapsed.

Feeds and Speed Calculator - Chip Load

$$Feed~Rate~(inches/min) = {Spindle~Speed~(RPM) * Number~of~Flutes * Chip~Load~(inches)}.$$

Chip load is usually between 0.001" and 0.010", with exact maximum chipload determined by end mill manufacturers based on the end mill and stock material characteristics, like surface speed. Most prototyping work on any material can be done well with a chipload of 0.005" for roughing passes and 0.002" for finishing passes. Even the sharpest blades have some roundness to the blade edge and just rub against the stock material before the pressure is high enough for it to start cutting. With the smallest chiploads (like 0.001" or even 0.002"), it is possible for the blade to just mash the material underneath and never create a chip, especially if the end mill is dull. If this happens, you must use a larger chipload to prevent overheating (including fire!), because a significant amount of the heat generated during the cutting process is ejected with the chips!

 Tool Diameter

Feeds and Speed Calculator - Diameter

Tool Diameter

Pocketing - to mill a pocket, you can save a lot of time by first "clearing" the majority of the material with a larger end mill and then running a second program to finish cutting the pocket edges that couldn't be reached by the larger cutter. To clear the pocket, you typically want to use the largest diameter tool that you have, which works with the material that you're cutting and fits inside the pocket. Then, use the largest diameter tool that works with the outline of the pocket for finishing, taking note of the minimum radius of the outline path that results.

Through cutting and profiling - a good rule of thumb is to keep the diameter equal to or larger than 1/6 of the material thickness, as this allows you to use full passes without having problems due to the end mill deflecting under cutting loads.

 Feedrate

Feeds and Speed Calculator - Feed rate

$$Feed~Rate~(inches/min) = {Spindle~Speed~(RPM) * Number~of~Flutes * Chip~Load~(inches)}.$$

Feed rate is the speed at which the machine moves the machining spindle across the part. The spindle speed is described here and the number of flutes is described here.

 Flutes

Feeds and Speed Calculator - Flutes

Number of flutes

For prototyping, you typically want to use as few flutes as possible, since this will clear chips (and heat) the best. This usually means one flute for low surface speeds (like for plastics) and two or three flutes for higher surface speeds. Higher surface speeds result in higher spindle speeds, making end mill weight and cutting load balance more important.

 Plunge Rate

Feeds and Speed Calculator - Plunge Rate

In general, a plunge rate should be less than 50% of the feed rate, due to typical end mill design. End mills are designed to cut more efficiently in lateral directions, rather than vertically (like a drill bit). Therefore, a gentler plunge rate helps to keep the temperature down and avoid damage to the tool. Remember that when plunge cutting, the surface speed will vary scross the radius of the end mill, all the way to zero at the very center. For this reason, all plunge cuts should be ramped - there must be some xy travel while plunging. This means that using a smaller diameter end mill to profile or pocket a vertical hole as a cutout will work much better than trying to drill with a larger end mill.

 Spindle Speed

Feeds and Speed Calculator - Spindle Speed

$$Spindle~Speed~(RPM,Revolutions~per~Minute) = {Surface~Speed~(ft/min) \over \pi * \frac{1}{12} * Tool~Diameter~(inches)}$$
 Step Down

Feeds and Speed Calculator - Step Down

The step down should be less than the diameter of the tool for soft materials such as plastics and wood. For hard materials such as metals, stepdown should be less than half of the diameter of the tool.

 tool diameter

Feeds and Speed Calculator - Step Over

The calculator sets the stepover as 45% of the tool diameter as standard however this can be changed depending on the geometric strategy used for pocketing. The maximum value you can use is 50% when rastering a pocket although we've found that 45% creates a better finish. When doing concentric outlines you are limited by the most acute angle in the outline (if it is 90 degrees then any more than about 30% (there's an exact number for this) will leave little uncut areas behind.

 Surface Speed

Feeds and Speed Calculator - Surface Speed

Surface speed is the linear speed that each tool edge will travel at, through your material while cutting. The maximum surface speed is determined by a combination of the nature of the material that you are cutting, and the nature of the material that your end mill is made of. Since end mills are typically quite expensive, you probably don't want to determine this experimentally. Most end mill manufacturers have done this work and publish lists of optimal surface speeds for various materials, using their end mills. For most end mill materials and surface coating combinations with the same description (eg. "titanium nitride (TiN) coated carbide"), maximum surface speeds are similar across manufacturers. Usually, the surface speeds listed by end mill manufacturers are maximum speeds, and it works well to cut at or below this speed (a few materials actually have a minimum surface speed for proper cutting, but this is relatively rare). You should start any new job at 50% (or less) of this maximum, in order to be able to observe any problems and pause the machine before a hazardous situation occurs - while surface speed is independent of feed rate in principle, using typical chip loads results in a tendency for feed rate to scale with surface speed.

The table at the bottom of the main page gives surface speeds for materials typically used in the Fablab, if you have any new materials that you'd like added to the table, or you think we should post different surface speeds then email gmpc at mit dot edu.

49.1 KB

67.1 KB

76.1 KB

97.4 KB

This diff is collapsed.
 #main { margin: 2em 5em; } h1,h2,h3,p,th,td,span,div { font-family: sans-serif, arial; } #tool_material_data { width:10em; } .myButton { background-color:#d0451b; border-radius:4px; border:1px solid #942911; display:inline-block; cursor:pointer; color:#ffffff; font-family:Arial; font-size:14px; text-decoration:none; height: 60%; text-align: center; } table td { padding:12px; background: #e0e0e0; background: -webkit-gradient(linear, left top, left bottom, from(#fbfbfb), to(#fafafa)); background: -moz-linear-gradient(top, #fbfbfb, #fafafa); text-align: left; } table tr { text-align: center; padding-left:20px; } table th { padding:21px 25px 22px 25px; border-top:1px solid #fafafa; border-bottom:1px solid #e0e0e0; background: #ededed; background: -webkit-gradient(linear, left top, left bottom, from(#ededed), to(#ebebeb)); background: -moz-linear-gradient(top, #ededed, #ebebeb); } table { border:#e0e0e0 1px solid; } .merged_row { text-align: left; } .lhs{ /*width: 100px;*/ float:left; display: table-cell; } .rhs{ /*width: 200px;*/ display: table-cell; padding-right: 1em; padding-left:1em; float:right; } .middle{ padding-right:1em; display: table-cell; } .equation{ margin:0 auto; display: flex; align-items: center; } .eq{ padding-left: 20px; padding-right: 10px; } #page{ text-align: center; } #diameter_flutes{ padding-left: 20px; } \ No newline at end of file
Markdown is supported
0% or
You are about to add 0 people to the discussion. Proceed with caution.
Finish editing this message first!