CNC Guide to Processing Quotes

• 1
  What a machining quote is actually made of
• 2
  Why material choice and tolerance class dominate cost
• 3
  Part geometry, access and volume effects
• 4
  How to read a quotation line by line
• 5
  What to send so the quote is accurate the first time
• 6
  Where cost can be removed without losing function
• 7
  Step by step: from file to signed quote
• 8
  How each input moves the price

A CNC quotation is not one number. It is a stack of smaller numbers: programming hours, setup hours, fixture cost, cutting time, material cost, inspection time, and the risk margin a shop adds for hard jobs. A high quote almost always means one of those lines is large, not that the shop is expensive overall.

Cutting time is the easiest line to estimate and the easiest to argue about. It scales with the volume of metal removed, the hardness of the workpiece, and the number of tool changes. A part that looks small on a drawing can still run 40 minutes of cycle time because it has deep pockets and thin walls.

Setup is where small orders get punished. Clamping a part once on a 5-axis center can replace three separate operations on 3-axis machines, which removes two setups and two chances of losing datum. On a 20-piece run that difference is visible in the unit price.

Programming and inspection are fixed costs. They do not shrink when the quantity drops. This is why the same part quoted at 1 piece and at 1,000 pieces can differ by a factor of four or more, and why the cnc guide to processing quotes always starts with quantity.

• 1
  VariableCutting time and material scale with the part itself.
• 2
  FixedProgramming, fixturing and first-article inspection do not.
• 3
  RiskTight tolerance and thin walls add margin a shop must hold.

Aluminium 6061 cuts fast with standard carbide and holds ±0.05 mm without drama. Titanium TC4 and Inconel 718 do not. They work-harden, they run at low surface speed, and they eat tooling. A part that takes 12 minutes in 6061 can take over an hour in Inconel, and the tooling cost is billed inside the cycle time.

Tolerance is a second multiplier. Holding ±0.005 mm on a feature usually means finishing passes at shallow depth, temperature-stable coolant, and a CMM check. Holding ±0.05 mm often means one pass and a caliper. The jump from one to the other can double the price of that feature, so tolerance should be applied only where it matters.

Surface finish behaves the same way. Ra 3.2 μm comes off the machine. Ra 0.8 μm needs a controlled finish pass with a fresh insert. Ra 0.2 μm may need lapping or polishing after machining, which adds a hand operation and a second inspection.

Stainless 316L and 17-4PH sit in the middle. They are machinable but gummy or abrasive, so feeds and speeds must drop. Brass C36000 and copper alloys machine faster than aluminium in some operations, but material cost per kilogram is higher.

A quote follows the toolpath. Deep pockets need long reach tools, and long tools deflect, so the shop must slow down. Undercuts and features on five faces need either a 5-axis setup or multiple fixtures. Holes with a depth-to-diameter ratio above 5:1 need peck drilling and sometimes a pilot drill.

Thin walls are a hidden cost. A 1.0 mm wall in aluminium can be machined, but the shop must control clamping pressure, use light finishing passes, and possibly add a soft jaw. Below 0.5 mm the part may distort during release and the quote must include a straightening step.

Volume changes the whole structure of the quote. At 1 to 10 pieces, the shop optimizes for setup time and uses universal fixtures. At 500 pieces it may build a dedicated fixture and write a probing routine. At 10,000 pieces it may ask about casting or die casting instead of cutting from solid.

No minimum order quantity exists at GreatLight, so a single prototype is quoted on the same line as a 10,000-part run. That does not mean the unit price is the same. It means the quote reflects the actual process chosen for that quantity.

A useful quote separates material, machining, finishing and inspection. If everything is bundled into one line, ask for the split. That single question tells you whether the shop priced the part or guessed at it.

Compare cycle time against part size. A 50 mm bracket quoted at 90 minutes of machining is either very complex or badly planned. Ask which feature drives the time. Engineers usually find one pocket, one tolerance, or one corner radius responsible for most of it.

Check the finishing line. Anodizing, electroless nickel and powder coating are outside processes with their own minimum charges, so they rarely scale linearly below a few hundred parts. Laser marking adds almost nothing if the character height is at least 1.5 mm and the file is supplied as vector.

Finally, look at what is missing. A quote without an inspection clause, without a material certificate reference, or without a note on who owns the fixture is incomplete. Those gaps become change orders later.

Send a 3D model plus a 2D drawing, not one or the other. The model defines geometry; the drawing defines which dimensions are functional, where the datums sit, and which tolerances are real. Shops that quote from a model alone will assume general tolerance and you will get parts that fit nothing.

State the material grade, not just the family. 6061-T6 and 7075 are both aluminium and behave nothing alike. 304 and 316L are both stainless and price differently. Grade affects both cutting parameters and material cost.

State the quantity you actually expect, including the ramp. If the first order is 5 pieces and the next is 2,000, say so. The shop can then quote the prototype on a bridge tool and plan the production fixture, which saves a second round of programming.

Mention critical features explicitly. If two bores must be concentric within 0.01 mm, write it. If a surface is cosmetic and must not show tool marks, write it. Everything not stated is treated as non-critical, and that is how disputes start.

• 1
  Model + drawingGeometry from CAD, intent from the print.
• 2
  Grade and temper6061-T6, 316L, TC4, not just the family.
• 3
  QuantitiesFirst order and expected annual volume.
• 4
  Critical notesConcentricity, cosmetics, mating surfaces.

Tolerance reduction is the fastest saving. Most drawings carry ±0.01 mm on every dimension because the designer never went back to loosen the ones that do not matter. Loosening five non-functional dimensions to ±0.1 mm can cut cycle time noticeably.

Corner radii matter more than people expect. A pocket corner that matches a standard end mill diameter, say 6 mm or 8 mm, is cut in one pass. A 5 mm corner in the same pocket forces a smaller tool, more passes, and a longer cycle.

Thread callouts should be standard. Metric coarse threads and unified coarse threads are stocked in every shop. Special pitches and left-hand threads need special taps and add setup.

Finishing should be applied only where it is seen or where it functions. Masking a cosmetic zone and leaving the rest as-machined is normal practice and usually costs less than finishing the whole part.