Guide
What is the difference between climb milling and conventional milling, and does it matter for your part?
Climb milling is milling in which the workpiece feeds in the same direction as the cutter teeth move at the point of contact, so each tooth enters thick and exits thin; in conventional milling the work feeds against the rotation and the chip starts thin and grows. Short answer: climb (down) milling is the general rule on rigid CNC machines because it makes less heat and gives longer tool life, while conventional (up) milling still has uses, such as some finishing passes on walls and older machines with lead-screw play. For a buyer the direction is the shop's choice; your drawing should control the result, not the method.
By Saola Manufacturing engineering team · Published · Updated
Vibration marks are covered in chatter marks in machining and thin walls that move after machining in thin-wall aluminum machining distortion. This page explains the two milling directions, what each does to the part, and what a drawing should say instead of prescribing one.
On this page
How do climb milling and conventional milling differ at the cutting edge?
The difference is the chip shape: in climb milling the chip starts at its maximum thickness and thins out, in conventional milling it starts from zero and thickens. That one fact explains most of the differences in heat, wear and finish.
A university machine shop guide describes conventional milling as starting with a chip of zero width, so the tool rubs more at the beginning of the cut, more heat goes into the workpiece and work hardening can follow; chips are carried up and can be re-cut, marring the finish. In climb milling the chip starts at maximum, more heat leaves with the chip, the tool rubs less and lasts longer, and chips fall behind the cutter (Washington University in St. Louis, student machine shops). MIT's machine shop notes put it simply: conventional milling feeds the work into the rotation of the cutter, climb milling moves the work with the rotation and produces a better finish, but is not recommended if the workpiece cannot be held securely or cannot support high forces (MIT OpenCourseWare 2.670, Mill).
The cutting forces also point differently. On a horizontal mill, conventional milling tends to lift the workpiece and climb milling pushes it down onto the table, per the same university guide.
Why is climb milling the default on CNC machines?
Because more and more machines compensate for feed-screw backlash, which made climb milling risky on old manual machines, and climb milling runs cooler with longer tool life. A tool maker puts the rule plainly: use down milling tool paths.
Sandvik Coromant's die and mold application guide states that down milling is normally more favorable because considerably more heat is generated in up milling, that tool life in up milling will generally be shorter, often as much as 50 percent, and that radial forces are considerably higher in up milling, which is hard on spindle bearings; in down milling the carbide edge is mainly in compression, which suits cemented carbide (Sandvik Coromant, die and mold making application guide, 2002). The Washington University guide adds the historical reason: conventional milling was traditional because it takes up the play between lead screw and nut, and climb milling became preferred as more machines compensate for backlash.
When is conventional milling still the right choice?
On machines with feed-screw play, and for some side-finishing passes on hardened material where wall straightness matters. The choice belongs to the process plan, not the drawing.
The same Sandvik guide makes two exceptions. When side milling (finishing) with solid carbide, especially in hardened materials, up milling is first choice because it is easier to get a better wall straightness tolerance and a more accurate corner angle; and up milling can be favorable on older manual machines with more play in the lead screw, because the counter pressure stabilizes the cut. Its example of end mill bending shows the effect: minus 0.02 mm in roughing and 0.00 mm in finishing for up milling, against 0.06 mm and 0.05 mm for down milling, in the conditions of that example (Sandvik Coromant, 2002). The MIT notes also describe conventional milling as needing lower forces and being preferred for roughing on the manual mills they cover.
For castings, which is much of the second-operation milling buyers send out, the trade-off is practical: as general shop practice, a hard skin or uneven stock may be hard on an edge that enters at full chip thickness, so shops may adjust the first pass, the tool or the direction. That is a tooling decision, and the right answer depends on the machine, the tool and the part.
What does the milling direction change on the finished part?
Surface finish, burr size and direction, how straight a thin wall comes out, and how hard the surface layer gets. All of these can be specified and inspected on the part, which is better than specifying the direction.
From the sources above, climb milling tends to give the better finish and less rubbing, while conventional milling can give straighter walls in side finishing because the tool is pushed away from the wall differently. Where a feature is thin or the tool is long, that deflection shows up as a tapered or out-of-flat wall, which is a geometric tolerance problem. Where the material work-hardens, rubbing at the start of a conventional cut can leave a harder surface that the next pass has to cut through.
Burr location tends to change with the direction and toolpath. If a burr would matter on an edge, call the edge condition on the drawing rather than hoping the toolpath puts the burr somewhere harmless.
| Concern | Milling effect | What to put on the drawing | How it is checked |
|---|---|---|---|
| Surface finish on a milled face | Climb usually finer; re-cut chips mar finish | Surface texture symbol with roughness value per ASME Y14.36 | Roughness measurement or comparison specimen |
| Thin wall straightness or taper | Tool deflection differs by direction | Flatness, straightness or profile tolerance per ASME Y14.5 | Indicator, height gauge or vision measurement |
| Corner angle and position of walls | Side finishing direction affects accuracy | Angularity, perpendicularity or profile per ASME Y14.5 | Angle and position check on first article |
| Burrs on edges | Burr location depends on toolpath | Edge break or burr-free note on named edges | Visual and touch check, magnification if needed |
Should a drawing or RFQ specify climb or conventional milling?
Almost never. Specify the surface texture, the geometric tolerances and the edge condition, and let the supplier pick the toolpath that meets them on its machines.
A process note such as “climb mill all walls” ties the supplier to one method without securing the result, and it can be wrong for a particular machine, tool or hardened material, as the Sandvik exceptions show. ASME Y14.5 gives you the tools to state what you actually need: flatness, straightness, profile and orientation tolerances on the walls and faces that matter (ASME Y14.5-2018), and ASME Y14.36 covers surface texture symbols for the finish (ASME Y14.36-2018).
If you have a real process concern, say it as a requirement in the RFQ: for example, that a sealing face must have no feed marks across the seal path, or that a thin wall must meet its flatness without stress-relief steps. The supplier can then plan direction, step-over and finishing passes to meet it and show the result on the first article.
How does Saola handle milling direction on your parts?
Milling runs at our lead CNC plant, mostly as second operations on castings; the toolpath is our process choice, and we hold it to the finish, tolerances and edge notes on your drawing.
The CNC milling page describes the work: mostly second operations on die castings and sand-cast brass and bronze, with simultaneous five-axis machining not offered; turned parts are on the CNC turning page. Inspection at the plant uses a 2D optical (vision) measuring instrument and a height gauge among other equipment. First-article inspection reports for new parts and a dimensional inspection record per lot are available on request, so wall flatness and angles can be listed as characteristics. Send the drawing through the quote form.
Frequently asked
Is down milling the same as climb milling?
Yes. Climb milling and down milling are two names for the same direction; conventional milling is also called up milling.
Why is climb milling dangerous on a manual mill?
Because of play between the lead screw and nut in the table drive, which conventional milling takes up and climb milling does not. The Washington University guide notes that more machines now compensate for backlash or have a backlash eliminator, which is why climb milling became the preferred approach.
Which direction gives the finer surface finish?
Climb milling usually gives the better finish, per the MIT and Washington University notes, but the finish you get also depends on the tool, step-over and rigidity. Specify the finish, not the direction.
Does milling direction affect tool cost on my quote?
Indirectly. Longer tool life in climb milling lowers tool wear per part, but the supplier balances that against finish and accuracy needs; it is part of their process, not a line on your quote.
Sources
- Die and mold making application guide (catalog 5747155), application technology section, Sandvik Coromant, 2002 (copy hosted by a distributor)
- 2.670 Mechanical Engineering Tools, Mill, MIT OpenCourseWare, 2004
- Climb Milling vs Conventional Milling, McKelvey School of Engineering Student Machine Shops, Washington University in St. Louis, accessed 2026
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018
- ASME Y14.36-2018, Surface Texture Symbols, ASME, 2018