You can set various general specifications for your part. For example, you can set the general tolerance, surface roughness, etc.
- Choose Job | Settings.
- Select any items on the left marked “Specifications”.
- Enter the desired settings.
- Click OK.
You can specify various general technical information about your part at menu Job | Settings | Specifications: Auto. These settings are described here.
Recommended settings for all items below are available by clicking one of the buttons at the bottom of the dialog. However it is best to select your own values depending on your specific requirements.
General Linear Tolerance
This setting specifies the permissible variation of certain measurements. For example the diagram shows a tolerance of +/- .005″ indicating that the length of the rectangle can be between 1.995″ and 2.005″. See Tolerances for details. For lowest cost select the largest acceptable value.
Material thickness tolerance
This setting specifies the permissible variation in thickness of 2D parts. For example, a tolerance of 20% applied to a 1/8″ thick sheet would mean that the sheet thickness used for your job could range from 0.1 to .15. For 3D parts, select N/A if you want the general linear tolerance (see above) to apply. If you select a percent value, the position of any holes or other features created on the edge of the sheet will be measured from the bottom side of the sheet in accordance with the general linear tolerance. It is usually more economical to use one of the percent values when parts are cut from sheets 0.75 in thick or less.
Due to limitations of manufacturing processes, edges (exterior and interior) that should be at 90 degrees to their adjacent surface cannot be exactly 90 degrees. This setting specifies the maximum deviation from 90 degrees that you will permit for edges perpendicular to the Top view. For lowest cost, select the largest acceptable value. Larger values reduce cost especially for 2D parts cut from sheets. For example, for a 1/16″ thick sheet and a 10 deg edge draft, the bottom side could have only up to .016″ more material at edges than the top side. (Tolerances will be applied to measurements on the bottom side.) If you select zero or Default for this setting, the job Tolerance setting will control.
This setting specifies how flat the largest outer flat surfaces will be. In particular, all points on those surfaces will be between two parallel planes the specified distance apart. For lowest cost select the largest acceptable value. For example, a potato chip might have a flatness of ~0.5″ and a business card ~0.1″.
These settings specify the smoothness of the surface (Top & Bottom views) and edge (Front, Back, Right, Left view), measured as a function of the height of the small ridges resulting from the cutting process. The setting you specify may be met by direct machining, polishing, sanding, grinding or any other method unless a specific method is specified. Examples: polished surfaces are often ~1 microinch. Machined parts are often ~63 to ~125 microinch. A phonograph record is ~250 microinch.
Note: Some manufacturing processes use multiple cutters, so where a cutter change occurs a minor surface discontinuity can appear. Such transition points will be held to a reasonable minimum for roughness settings 63 and smaller. Minimizing such transitions is usually appropriate only for highly visible parts where appearance is a prime concern.
Tolerance is a specification for how much variation from ideal measurements you can tolerate for your parts. You must specify a tolerance in menu Job | Settings. If you are new to thinking about small tolerance values, consider the thickness of some common items:
- Copier paper ~.003″
- Business card ~.014″
- Credit card ~.030″
- House key ~.080″
Note that metals allow for parts of tighter tolerance than plastics.
For specific tolerance limits please click here.
You can specify tolerances in three ways:
- To set the general default tolerance select a value from Job | Settings | Specifications Auto | General Linear Tolerance .
- To set a tolerance for a specific feature (e.g. a hole diameter, a length, etc): draw a straight line across the feature and select Line | Machine | Tolerance:
Vague Tolerances Vague tolerances are not accepted, such as, “The diameter must be exactly 1 inch.” Or, “This dimension is critical.” Or “Size must be accurate.”
Implicit and Explicit Tolerances
Often, mechanical drawings show lines with arrows and other symbols that indicate distances and other measurements that must be held to a certain tolerance. For
eMachineShop CAD offers the ability to rely mostly on implicit dimensioning which is easier and faster to use. Implicit dimensioning is supported via the general tolerance at Job | Settings | Specifications.
The linear tolerance value you specify at Job | Settings | Specification is referred to below as “T”. In simple terms, the value you select for T is used approximately as follows:
- The size of features such as circles,
slotsand outer shapes can vary by +/- T.
- As measured from datums, the center of circles can be in a circular region of radius 1.4* x T.
- As measured from datums, the position of single straight edges can vary by +/- T.
See below for the precise rules.
Allowance for finishes
In conformance with industry standard, design dimensions are after non-organic and mechanical finishes (anodize, electroplate, brush, grind, sand blast etc.) but before organic coatings (powder coat, etc.). Example: A 10 mm cube that was electroplated should measure 10 mm after electroplating.
Below is the complete definition of how default tolerance is used at eMachineShop, requiring an understanding of GD&T and ASME Y14.5. The following is used as the basis for determining whether your part conforms to your specification:
Additionally, tapped holes shall be perpendicular to the originating surface within +/- 2 degrees.
The general tolerance does not apply to
Following is the order of precedence of tolerances with
- Tolerances indicated via Comments To Machinist.
- Local tolerances from the Line | Machine dialog.
- For 2D parts cut from sheets Job | Settings | Auto: Specifications | Material Thickness Tolerance – applied to sheet thickness only.
- General tolerance per Job | Settings | Auto: Specifications | General Linear Tolerance.
For parts made by extrusion the general tolerance applies to the cross-section.
Tolerances may not be met when impractical due to
Measurements are done at at 20C +/- 1 or 68F +/- 2.
* The value 1.4 (SQRT(2)) and 2.8 (2 * SQRT(2)) are derived from the GD&T equivalent of older style square zone tolerancing where +/- T is applied separately to each axis.
eMachineShop will generally accept tolerances down to:
Machined 2D parts
Overall sizes and positions: +/- .01″
Local cutout sizes: +/- .005″
Local diameters: +/- .002″
Machined 3D parts
Overall: +/- .005″
Local pocket and protrusion sizes: +/- .001″
Local diameters: +/- .001″
For injection molding, rapid prototyping and other non-machining processes please see the respective web pages.
Also see tolerances.
The eMachineShop CAD software uses implicit dimensioning which means that you don’t have to spend the time creating conventional dimensioning lines. However, numerical positions, diameters and similar information is visible in the numeric bar (located under the toolbar) upon clicking on a line.
Nevertheless, if desired or needed, you can specify or annotate dimensions directly on your drawing.
To add explicit dimensions to your drawing:
- Draw a straight line.
- Choose Line | Machine.
- Choose Comments to Machinist (or) Comments To Myself | Dimension. Or for tolerances choose Tolerance from the left pane.
- Click OK.
- If the dimension line overlaps a line on your original design, nudge the line a bit away from the original line.
Allowance is a provision to allow for deviation between an actual dimension and an ideal dimension.
For example, suppose you need a hole for a 1/4″ bolt. It is a common error to simply draw a 1/4″ circle. Unfortunately you may receive your machined parts and find the bolt does not fit! The reason? No hole is exactly 1/4″ – all manufacturing processes have variation and this is controlled by tolerance. If the tolerance is +/- .01″ and the hole is at the low limit of .25 – .01 = .24, the bolt may not fit. To prevent this draw the circle at diameter .26. Then the low limit will be .26 – .01 = .25 which would clear a 1/4″ bolt.
Similarly a 1/4″ shaft that must fit inside a 1/4″ hole should be designed to be sure the shaft can be inserted. For example, if tolerance +/- .005 is used for the shaft and hole and you set the shaft to .245 and hole to .255, at the tolerance limits the actual shaft could be as large as .250 and the hole as small as .250 so they will still fit. However such a fit might be tight so you might add .001 or so to the hole or subtract from the shaft to insure that the fit is loose. Then you would specify a shaft of .244 and hole of .256. You should also think thru the opposing limits. The hole could be as large as .261 and shaft as small as .239 leaving a gap of .022. If that is too loose you would need to tighten the tolerances.
The foregoing are just simple examples. You, the designer, are responsible for allowances, to be sure your parts fit and work properly.
When designing and ordering custom manufactured parts you must exercise great care to specify exactly what you want. We want you to be happy with your parts!
Specify everything that is important
The eMachineShop CAD software helps you specify many common aspects of designs but you must add any additional requirements you might need. Manufacturing and mind-reading don’t mix. For example: among the endless possibilities, here are a few of the more common factors that you might need to specify:
- Local dimensional positions – for example you might need to specify that the center to center distance between two holes is 1.000″ +/- .003.
- Local dimensional sizes – for example you might need to specify the diameter of a hole is 1.25″ +/- .002.
- Other GD&T factors such as Angularity, Perpendicularity, Cylindricity, Runout, Parallelism, Straightness, Concentricity, Circularity, etc.
- A particular color
- A specific texture or appearance of the surface finish
- Dimensional tolerances of parts after bending is applied – for example the distance (with tolerance) between legs of a U shape bend.
Of course you must also pay attention to all the settings presented in the CAD software and all warning messages.
Make sure you specify every important detail about your job! eMachineShop cannot accept rejections based on specifications you never communicated.
Datums, described in more detail here, are locations on a part that indicate a “base” from which measurements are taken. You can specify datums for your design but are not required to do so.
- Draw a straight line.
- Apply menu Line | Machine | Datum.
- Use Comments To Machinist text to label each datum (usually A, B, C).
- Generally, 2D parts have 2 datums and 3D parts have 3.
Process permissions allow you to specify which types of additional special manufacturing processes you will allow, or require, when making your part. Special processes you allow will be used only when cost (or time) effective. For example, enabling Molding/Casting means your job will be molded or cast only if it saves you money or time. Processes you require will be used unconditionally. If you uncheck all special processes only conventional processes will be used.
Additive extrusion – Forms your part by CNC controlled extrusion of a .01″ to .02″ diameter plastic extrusion. This process builds up your part layer by layer. This results in a permeable material that is not recommended for holding liquids or gases. (Generally recommended only when very fast delivery is required.) Be sure to see the details of this process.
Molding/Casting – Forms your part by molding or casting. These processes create a slight line where mold sections meet and where ejection mechanisms push the workpiece from the mold.
Manual machining – Allows for non-CNC machines to be used. This may lower cost for very simple parts at very low quantity, at a slight sacrifice in surface uniformity.
Secondary processes for intricate thru cutouts – When you have cutouts that go fully thru your part and have sharp or small radius corners, the analyzer might advise you that some of the material might not be removed due to the limitations of conventional machining. With this option you can request that extra steps be taken to remove such material (at higher cost).
If you are new to custom manufacturing, it is important to understand who is responsible for what:
- eMachineShop’s responsibility is the create your parts to meet the drawing and explicit specifications included in your orders.
- Your responsibility is to create designs and specifications that meet your desired need and functionality.
For example, if you specify 1.0 +/- .005 for the size of some feature on your part, it is eMachineShop’s responsibility to make the size between .995 and 1.005″ but it is your responsibility to make sure that all values within that allowed range will fit your motorcycle or cold fusion energy invention.
Make sure you include all relevant specifications – any design elements that require a specific tolerance or specific look etc. must be specified precisely in your design.
The following specs apply to bends:
Linear bend position – limits variation of the position of the center of a bend – that is where the male punch contacts the flat sheet – only for bends directly adjacent to an edge.
Angle tolerance – limits variation of angle after the part is bent.
Radius of bend tool – actual radius of the male punch tool. The inside radius on the bent part will usually be a little larger – how much depends on the thickness, material, etc.
Die width – this does not influence the radius or angle of the bend – generally use the smallest value that does not give an error.
Minimize bend marks – reduces visibility of marks caused by the bending process.
Generally you should use the Model Bends command to estimate the results of a bend.
IMPORTANT: Note that dimensions between features on parts after bending can vary substantially due to an accumulation of tolerances, especially on complex bends. You must use Comments To Machinist to specify any needed tolerances such as the distance between two legs, the distance between holes after a bend, etc.
When designing and ordering custom manufactured parts do not rely on the outcome of prior orders. Each order must stand alone and specify all details independently of other orders.
Just because a prior order met your expectation or functioned correctly does not mean a reorder will do the same. Tolerance controls conformance, not prior orders. There will always be some variation from one order to the next due to machinist preferences, process changes, wear of cutting tools, variations in methods, etc. The purpose of tolerances is to specify an allowable range of variation. This applies to all the specifications in your order.
For example, suppose you place an order for a part with a 1″ hole into which you plan to insert a shaft. And suppose you set the general tolerance to +/- .005. On a first order all the holes might, by chance, range from 1.001 to 1.005 and the shaft fits through. On the next order some or all of the holes fall into the range .995 to .999 and the shaft does not fit. The parts are in spec but non-functional. It is your responsibility to specify tolerances so that your part will function throughout the tolerance range. In this example you might have needed to specify a hole size of 1.006 +/- .005.
As another example, suppose your first order has parts with a surface texture or appearance that you like. Then you follow up with an order that has a different surface texture or appearance. Both orders will be considered in spec unless you specified a specific texture or appearance that was not met.