Why Center-Tolerance CAD Models are Important for Production Engineering

Autodesk Support

Aug 9, 2019


Production engineering often uses CAD-based computer-aided manufacturing (CAM) systems. While technical drawings are meticulously prepared, CAD models often lack production information, such as manufacturing tolerances. Production engineering needs so-called center-tolerance CAD models to start producing without further ado. Together with other options, this article outlines the best practice to derive center-tolerance CAD files with Autodesk Inventor.

Introduction

Manufacturing data mostly relates to the overall list of parts, technical drawings, and CAD data. The latter is becoming more and more important since computer-aided manufacturing (CAM) systems are widely used in modern production and they require 3D models to generate NC code for machine tools.

While there are exist standards for technical drawings, the baseline for CAD data communication is unclear. Often, design departments forward CAD models and technical drawings to production engineering and CAM system users. The reason behind is that CAD models don't hold all required manufacturing information. For instance, they lack information on general dimensioning and tolerancing (GD&T). Hence, production engineers use CAD models for CAM, but still have to check corresponding drawings for surface qualities and manufacturing tolerances.

Asymmetrical Tolerances & Center-Tolerance CAD

One implication of CAM is that it generates NC code based on geometric information CAD, which is commonly created with nominal dimensions. However, if asymmetric tolerances are specified, a nominal-dimension CAD model doesn't contain the dimensions to manufacture to.

Assume a slot with a nominal width of 35 mm and tolerance +0.5/+0.2, to ensure it can fit an adjacent part. The slot’s min. and max. manufacturing limits are 35.2 mm and 35.5 mm, respectively. This slot’s tolerance field is asymmetric in relation to the nominal dimension, and if it were manufactured exactly to the latter, it would require rework. Another example of an asymmetrical tolerance field is +0.2/−0.1, so – of course – the nominal dimension can be part of the tolerance field.

To eliminate rework or waste, parts should be manufactured to center dimensions. For our slot, this is 35.35 mm, which equals the theoretical center of the tolerance field. This will reduce the risk of finishing the dimension out of tolerance, given that a machine tool's production tolerance scatters. Concerning fittings, it should be noted that virtually all tolerances specified by ISO 286 standard, e.g., “H7” or ”f8”, are non-symmetrical.

In the following, various ways to obtain center-tolerance CAD files and handling asymmetrical tolerances with Autodesk Inventor and Inventor CAM are discussed.

Using CAM

One common way to manufacture to center tolerance is through modifications in CAM, which is associated to production engineering. Two often-reported, easy ways are shown in Figure 1. What makes them so easily is that they work with CAD data from any source.

To obtain a CAM toolpath that follows the center dimension, either tool or part offset are modified to match the respective tolerance. For out slot, tool offset (radius) would be modified by −0.175 mm (−0.35 mm/2) to offset the resulting toolpath such that it hits the center dimension of 35.35 mm. The same principle applies when the part offset is modified. Nevertheless, both methods require user calculations and are non-adaptive in case CAD geometry or tolerances change – a potentially large source of mistakes and rejected parts in production.

Figure 1: Obtaining center-tolerance NC code through modifications in CAM, no adaptivity and a possible source of mistakes.

Using CAD

Because center-tolerance leads to non-nominal manufacturing dimensions, it seems more natural to account for their geometrical ramifications in CAD, that is, before CAM systems are involved. In Autodesk Inventor, there are three ways of going about center tolerance, which also depends on the original CAD data source (see Figure 2). Unsurprisingly, working with native Inventor files offers the widest range of possibilities, but third-party files can be processed as well.

Figure 2: Ways to create center-tolerance CAD models in Autodesk Inventor.

The first way to include asymmetric tolerances is to directly alter feature dimensions in Autodesk Inventor. Nonetheless, this approach has the same drawbacks as modifying offsets (CAM, Figure 1). It should not be used in a business environment, because it involves changing original CAD data.

The second, slightly more elegant option is to make use of Inventor’s “Direct Edit” feature. It allows for offsetting surfaces or hole dimensions. Even though it cannot offer adaptivity with tolerances, it adds an offset feature to the CAD feature tree and, hence, makes such changes traceable and easy to suppress. In addition, it can be used with non-native Inventor files, e.g., STP or CAD data from third-party software through AnyCAD. This method is passable when external CAD files need to be processed in CAM, but should be used with care; especially if changes are made to the original CAD files.

The third and undoubtedly best option is to directly attach tolerances to feature dimensions. This is demonstrated in the video below. Autodesk Inventor allows defining tolerances at the sketch-level or for feature dimensions, such as extrusion distance. The resulting CAD model can easily be switched forth and back between nominal dimensions and center dimensions, using parameter management.

Video: Attach tolerances to dimensions and easily control nominal dimension/center-tolerance. The model in the video also has Autodesk Inventor’s model-based definition (MBD) assigned, to enrich CAD with product and manufacturing information (PMI), like surface roughness or general dimensioning and tolerancing (GD&T).

Moreover, the model geometry status (nominal, center) can be accessed by iLogic (Autodesk Inventor API). This is particularly useful for workflow automatization, where CAM toolpaths should be updated based on a center-tolerance CAD or such models should be generated automatically. It becomes clear that this option not only allows to simply select the desired dimension status but that CAD model dimensions will adaptively update when tolerances change. The benefits for downstream processes are that center-tolerance CAD models can be created effortlessly. Furthermore, tolerances are directly accessible from the CAD model and, together with model-based definitions, this is an important step towards digitizing manufacturing information.

Summary

This article briefly outlined how CAD data are consumed by production engineering and CAM systems. Center-tolerance models are a best practice to providing CAD data for manufacturing and there are several options to create or derive them. The best practice for native Autodesk Inventor is attaching tolerances to dimensions. As a result, center-tolerance CAD models can be derived by simply switching the dimension parameter status from nominal to center-tolerance. Thus, there is little to no overhead for design engineers. In addition, production engineers get exactly the data they need to start converting the digital product into a physical one, without further ado.

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