CNC machining services start from $59 USD per order. Save on projects with our quantity discounts! We calculate quantity discounts based on several factors including part size, material, and overall design complexity. Our app will automatically provide discounted pricing for qualifying parts before checkout.
Turnaround for CNC milled parts is 3-7 business days before shipping, and our pricing system will show an estimated lead time while you build your cart.
Minimum overall part size: 1” x 1” x 1”
Maximum overall part size: 7” x 7” x 12”
We offer 6061 T6 Aluminum for CNC machining services. More materials coming soon.
| AutoCAD | .step, .stp |
| Inventor | .step, .stp |
| Fusion | .step, .stp |
| SolidWorks | .step, .stp |
If there’s trouble uploading your finished file to our pricing system, please ensure your design meets all requirements listed in these guidelines.
At SendCutSend we have the following capabilities for CNC machining:
We can produce dimensional features including pockets, slots, holes, bosses, webs, and flanges of varying heights and thicknesses.
Only include one modeled part per file to ensure your part is priced accurately. Do not upload assemblies.
Design your parts exactly as you want them milled in 1:1 scale.
Our system recognizes inch and millimeter units only. Use either inches or millimeters when designing to ensure your overall part size is interpreted correctly.
Only include one solid body per STEP file with no extra meshes, surfaces, or sketches. Do not model threads.
If extra faces or surfaces are left over from early iterations of your design, delete them from your model. Unnecessary faces will increase machining time and could result in a poor surface finish.
We guarantee +/- .005” overall accuracy or better.
This means that the size of a feature can be .005” bigger or smaller than designed and can also vary in position by .005”. Therefore, milled feature size can vary by up to .010”.
We do not offer specialized or custom tolerancing for milled parts at this time.
We’ll produce your parts based on the model you upload.
There’s no need to provide supplementary technical drawings with callouts. Drawings/prints will not be referenced.
The minimum internal machined cutout size for CNC milled parts is .125” or 3.175mm. This means the minimum internal radius we can produce for machined features is .0625” or 1.587mm.
Our smallest drill is .0629″, so we can produce circular holes as small as .0629″ (1.597mm).
Due to the cylindrical shape of the CNC mill’s tooling, sharp internal corners won’t be producible.
The minimum internal radius we can produce will be .0625” or 1.587mm.
Similar to our CNC routing service, outside corners can be sharp while internal corners will be radiused.
Any features with concavity should be considered “internal” features.
Since CNC machining is a subtractive process, enclosed hollow features and undercuts are difficult for our tooling to reach and may not be producible.
To visualize machinability for a part you’re designing, imagine your finger is the cutter. You can use the sides of your finger to profile walls, and the tip of your finger to mill floors or drill holes. Although you can move the part through various positions to reach additional sides, you cannot bend your finger to access blocked areas.
Tapping, threading, and anodizing (black and clear) are available via our Support team.
Follow our guidance to save time and money on your CNC milled projects.
There is no minimum feature depth.
Holes up to .500” in diameter are likely to be drilled features. We recommend that circular holes up to .500” in diameter be sized consistently with standard drill indexes.
As a rule of thumb, holes that are up to .500” wide can have a depth that is up to 8x the hole’s diameter. For example, a .125” (3.175mm) diameter hole can be up to 1” (25.4mm) deep.
Hole sizes exceeding .500” will often be predrilled and interpolated to achieve the final hole size. For holes or cutouts over .500”, the maximum allowed depth will typically be up to 4x the hole diameter.
Standard hole sizes may be eligible for greater depths depending on the part’s overall design.
Slender, unsupported geometry is most susceptible to warping and deformation during the machining process. Sufficient wall thickness in your design should prevent parts from being too fragile or likely to vibrate while being machined.
We recommend that wall thicknesses be at least 1/8th of the wall height. Greater wall thickness allows for less deflection, more repeatability, and better surface finishes.
Wall profile and supporting geometry greatly impact a wall’s rigidity. Standalone walls are more likely to have poor surface finishes if the wall height is just 4x the wall thickness, while supported types (curved walls, tub-walls, webbed walls) can maintain rigidity with heights up to 10x the wall thickness.
In specific instances, thinner wall features may be producible if the cutting load is parallel to the wall and can be cut with a slitting saw (for example, a heatsink fin).
Internal wall-to-wall corners will require a fillet which is at least the radius of the cutter being used, or at least one fifth the height of the wall – whichever is greater.
For example, a 1” deep pocket should have a fillet with at least a .200” inch radius in the corner between walls. The tool can sweep the profile of the pocket to accommodate any radius larger than the tooling, and these corners do not need to be “on-size” for the tooling.
A fillet with a larger radius will generally make the part more manufacturable, as it allows a larger and stronger tool to fit into the corner.
We may substitute floor radius cutters for the nearest size available if needed. This will have minimal impact on your finished parts.
When possible, wall-to-floor corners should be orthogonal or 90 degrees to give the tool consistent access to the floor and wall.
Wall-to-floor corners should be sharp. This allows the floor and wall to be finished with a single pass.
Alternate sizes can be produced, and in some instances will be required, but designing to match our nominal sizes will give you faster turnarounds and produce a more consistent finish.
In instances where the wall-to-floor corner is non-orthogonal (not 90 degrees), a larger radius should be used to allow the tool access to all surfaces of the part.
Multiple fillets or other 3D features require the use of a ball-end mill for finishing. These toolpaths take more time to complete because the tool has to be smaller in diameter than the smallest feature being machined and must be stepped over (or down) in much smaller increments to create a smooth surface.
Time consuming features will typically increase a project’s cost. If cost efficiency is important, consider reducing the amount of 3D features in your part if possible.
If you leave sharp edges in your model we’ll provide .010” (.254mm) edge breaks by default.
Alternatively, you can model a .060” / 1.5mm radius fillet on edges you’d like softened. This will cost less than fully rounded edges while giving you a similar effect.
Now that you have the knowledge you are ready to start designing your parts for the CNC machine. Questions? Reach out to our support team.
