Procnc - Design Guide For Cost Effective Machined Parts - I

Design Guide for Cost Effective Machined Parts: Engineers can affect the cost of parts they design. This may seem like an obvious statement but the difference between a design that is easy to manufacture and difficult to manufacture can sometimes be very subtle. Nowhere can this be more true than with parts that are manufactured by CNC machining. Engineers often don’t possess the on-theshop-floor experience that it takes to maximize every aspect of their design to be as cost effective to make as possible. This is where we come in. We see thousands of designs every year, and nearly all of them can be optimized from one degree to another. The following is just a sample of suggestions that we often give to engineers in order to make their parts less expensive to machine. Additionally, this document outlines some design suggestions or factors that drive the costs of machined components. It will help the engineer make choices during the design process which may reduce the cost of the end product. Choosing Materials: When choosing materials, allow the use of different forms of the material such as bar stock and plate. There can be significant differences in the cost and lead time of acquiring different forms. The Table below shows approximate $/lb and machinability ratings for common metals. Consider the strength vs. machinability rating as well when choosing materials. Choosing an annealed but heat treatable alloy of steel for example and then not specifying any heat treat will just drive cost with little benefit in material performance. As you see below, some aluminum can have even better performance than some grades of steel with significantly better machinability.

Price can be significantly affected by the total weight being purchased and cut sizes, and these prices below assume a decent amount of material is being purchased. Geometry Considerations:

Figure 1: Short and Rigid tool can cut this.

One of the single biggest cost drivers for machined parts is the length of time it takes to machine it. The rigidity and strength of the actual cutting tools often determines how much time it takes. Very simply, the shorter a tool is, the faster it can feed, and the less the part will cost to make. The selection of these cutting tools is determined by the design of the part and a few simple rules can really help reduce machining time. When designing parts that have pockets, or other features with vertical inside corners, you will need to leave a radius as the machining process uses rotating tools. Use the largest radii you can get away with. The tool that is used to machine a particular feature will obviously have a diameter of 2x the radius that you put in your model. If you design a part with a 1/8” radius, it will require a minimum of a 1/4” tool to cut that feature.

Figure 2: Long and flexible tool needed.

The larger a tool that can be used in that corner, the faster it can feed through the material. As the length of that corner increases, the length of the tool must increase as well and that tool must be fed much more slowly to avoid deflection and breakage. The relationship is worse than linear. For every doubling in length, the feed-rate is more than cut in half. When figuring costs, assume that a double of the ratio equates to a double of the cost of that feature. A good ratio is less than 3:1. Once you get up to 4, 5, or 6 to one,

the feed-rates are much slower. See figures 1 and 2. Under normal circumstances, 8:1 is the upper limit and is very slow and expensive to cut.

Figure 3: Virtual sharp or small corner radius

By using these simple guidelines, significant savings can be achieved in the cost of your machined parts. Sometimes you just need to have a long small radius because of assembly issues. There are still options to reduce the cost of features like this. Figure 3 shows how you can make a virtually square corner with very little intrusion into the surrounding walls. This is a great technique if for weight or assembly reasons you can't tolerate a larger radius. The key to this feature is to not put the center of the radius on the intersection of the inside edges. Put the center point inboard and then you can adjust it to fit your application. Use the biggest radius that fits the application as well.

Figure 4: Equal Radii on floor and wall costs 10X.

It isn't uncommon for engineers to put a radius both on the floor and wall intersection as well as the vertical walls (see fig 4). With the "apply round" or fillet feature on most 3D CAD systems, the easiest thing to do is to select both that floor intersection and the wall intersections and just apply the same size radius to all those. But in fact, what saves you a few seconds work to have just one feature, can cause enormous headaches for the machine shop and cost you a lot of money in the long run. It isn't obvious what it takes to machine the area in the corner. It is much more complicated if the floor radius is smaller than the wall radius. Because of the equal wall and floor radii, two tools must be used to clean up this area completely. The wall needs to be cut with a ball end mill (an end mill with a full radius on the tip). The floor of the part needs to be cut with a flat end mill, but this will leave a triangular shaped section in the corner that neither tool can reach. (see fig 5).

Figure 5: Material in blue is hard to remove.

This condition can be avoided by modeling the floor radii smaller than the wall radii (see Fig. 6). This enables the shop to machine this entire area with one tool that has a flat bottom but also has radii on its tips. In the last issue of Pro Tips we identified that the larger the vertical corner radii can be, the faster the tool can travel and the cheaper the part will be. Generally speaking the smaller the floor radii can be, the better, with a 0 radius being the easiest of all. In the US, tools are readily available with tip radii in .01" increments up to .125". And when indicating a tolerance of this floor radius on your drawing, make it as generous as possible to allow the shop greater flexibility in choosing tools. To put it into perspective, the equal corner radii detail will easily cost 10x what the unequal corner radii detail costs. That should offer enough incentive to spend a couple extra minutes modeling the optimum radii on your part, and reap the benefits for the life of the part.

Figure 6: A larger wall than floor radius is much faster to machine.

Material Shape and size: The size and shape of your part is nearly always driven by the function. Sometimes the constraints are hard and fast but other times you have some flexibility to design the outer size and shape. There is a good opportunity to design out some cost by considering what size material the part might be made from. We already saw above in the material table, that if available, bar stock is always cheaper than plate material. When bar stock is chosen as a material option, it is best to consider what size stock your part might fit into.

Figure 7: This part could be cheaper if it were a little thinner.

In Fig. 7 we see a part that is .74” thick x 3.3” wide. This part fits nicely into bar stock that is 3.5” wide, but it isn’t quite thin enough to be made from .75” material. With only .01” clearance between the part and material we can’t guarantee the tolerances and clean up the faces. In this case, we have to use 1” thick material which costs 25% more and spend time to remove extra material as well. If the part could have been designed at a maximum thickness of .65” or less, it is likely that .75” material could have been used.

There are some creative methods of minimizing excess material. For smaller parts that get clamped in a vice, .05” is probably about the minimum amount of excess that is needed. For very large flat parts that are held down with fixtures, occasionally even less can be left. If you are unsure, consult your manufacturer early on in the design phase where changes cost the least amount of money. Occasionally, designing a part to be exactly the size of the raw material can be done if the tolerances and cosmetic requirements are very low and "stock" surface and tolerances are expected. If you need to have all sides finish-machined, a safe rule of thumb is to leave approximately .1" on the length and width and at least .125" on the thickness. The side the thickness would be measured along would be the one where the primary material removal is occurring. With some designs, it isn't clear which way the part would be machined and it is prudent to engage the machine shop early on for advice on where they will need to hold onto the raw material, and how much of it they will need when they machine it. Tolerances Nothing can drive up costs on a part more quickly than tight tolerances that are difficult to machine or measure. Some tight tolerances are not any problem at all to achieve, while others are very challenging. All too often we see drawings with poorly applied tolerances which drive up the cost of the part or worse, potentially not fitting together with its mating parts. A better understanding of the machining process will allow the engineer to specify an intelligent tolerance scheme which serves their needs well but doesn't needlessly drive up costs.

Figure 8: Faces on the same side are easier to hold tightly.

As a rule of thumb, features that are created by the machine tool capability will be relatively easy to hold to a high tolerance. On the other hand, features that are affected by operator handling and loading into subsequent fixtures will be much harder to hold at a high tolerance. An obvious example of an easy to hold tolerance is the dimension between two steps on the same side of a part as seen in Figure 8. The same tool will be

used on these faces and the positional accuracy of the CNC machine will be the primary contributor to variability (essentially zero). With a positional accuracy of around .0001" [.0025mm] on an average CNC machine, this should be much tighter than most applications require. So if you need to specify a tolerance of .002" [.05mm] this shouldn't pose too much of a problem. Conversely, if you need to specify a high tolerance to the opposite face of the part, like in Figure 9, this would be much more challenging. The reason for this is because in most cases the part will be removed from the CNC machine, manually flipped upside down and re-clamped in order for the back side to be machined. There are a lot of variables introduced with this process and a tolerance of .002" [.05mm] would be much harder to achieve. There would likely be more complicated fixturing, longer machine set-up, longer loading times per part, and a higher scrap rate. These would all drive cost considerably. Given the above, parts will still generally be less expensive to make when tolerances are looser. Often engineers rely on the tolerance block to help communicate their needs such as .xx = .01" , .xxx = .005", .xxxx = .001" (or metric equivalent). Sticking with these general tolerances is easy to specify but may drive cost needlessly. If .005" is too loose of a tolerance, it doesn't mean that .001" is the only other option. Why not specify something in the middle, such as .003" or even .0035"? An intermediate tolerance may be much easier to achieve and subsequently less expensive. When working with smaller tolerances, a small difference can be vastly easier - .0015" is 50% more tolerance to work with than .001". Depending on the application, that extra .0005" might make the difference between hitting your parts cost budget or not.

Figure 9: Faces on opposite sides are more difficult to hold tightly

With every application there is a point of diminishing returns where loosening up the tolerance won't lower the cost of the part. If the process employed to make the feature can easily hold the tolerance, then making it looser will not reduce price, unless it becomes loose enough that a different and less expensive process can be used. For example, a part's tolerances could be loosened enough that it becomes feasible to use profiling technology like laser cutting, abrasive waterjet, or routing. You may also consider the option of supplying a mating part for an in-process fit check. It may also be sufficient to perform a "program check" where the programmer verifies that the feature will match the

model but there is no physical verification done. Discussing specific applications with your manufacturer is the best way to determine if changes might apply in your application. It is becoming common to apply a global profile tolerance to an entire part. While easy to specify, this may require significant inspection costs to prove. Even if a part does fall inside a profile tolerance, the manufacturer would need proof of that being the case. This would require a significant number of hand measurements or a full CMM report, either of which is costly. While profile tolerances have a real purpose, be sure you are using them effectively. Other geometry considerations: 1. On outer corner edges, chamfers are less expensive to machine than radii. Radius tools are more difficult to adjust so they are perfectly tangent on top and bottom. 2. When designing angled walls, choose .5 degree increments for shallow angles (.5, 1.0, 1.5 deg.) and 5 degree increments on larger angles (30, 45, 50, etc.). On pockets that have drafted surfaces, apply the radius to the wall intersection and then apply the draft. This is much less expensive to machine than if the draft is applied before the radius is put on. 3. When specifying engraving or machined part marking, only place it on surfaces which will be machined with the end of a tool and already will have an operation from that side. You want to avoid creating the need for another work holding just to machine the part marking. 4. When designing a feature that needs to be undercut with a relieved end mill or t-slot tool, be aware of the ratio of the cutting portion and the neck size that needs to support it. The smaller in diameter the neck needs to be, the more fragile it will be and the slower it will need to be fed. There aren’t hard and fast rules for this so discuss the feature with us during the design phase. 5. When designing narrow slots, chose a width that is slightly larger than the standard 1/16” increments that cutting tools come in. That will allow a roughing pass down the middle of the slot and then a finish pass around the edges so the surface finish is better. Helicoils vs. PEM studs vs. nothing at all. If needing to design some female threads into a part, consider if it can be just threaded into the base material or if it requires a stainless or steel insert. If you have enough room for at least 2x thread engagement, and the fastener will not need to be removed and reinstalled often, then just tapping the base material will offer plenty of strength. In a good grade of aluminum for example, a steel fastener will typically fail before the threads will pull out if there is more than 2x the diameter of thread engagement. If it is determined that you do need a stronger thread, consider whether or not a helicoil insert or a PEM stud would be a cheaper option. In most cases, helicoils are a better choice. They

are less expensive to buy, are faster to install with fewer installation failures, and they have better serviceability if they ever need replacing. PEM studs can be a great option if you need your threads to protrude up above the top of a part where they are the only feature above the face of the part. You may be able to start with thinner material and install a tall female threaded PEM stud rather than machining away a lot of excess material to leave islands of material that then get tapped with a helicoil installed. Drawings There are lots of potential pitfalls when creating 2D drawings that can inadvertently drive cost. Here is a short list of things to do and not do: 1. Use good zero reference points for all dimensions. Don’t dimension to tangent points of radii, theoretical points, intersections of obtuse or acute angles, or any other feature that is hard to establish. 2. Don’t choose a symmetrical tolerance where there is no obvious center reference point. 3. Ordinate dimensions are pretty easy to understand and to measure for things like hole patterns. 4. Don’t over dimension your drawing by dimensioning every possible feature. Minimally dimensioned drawings are much less costly to inspect. Features that are established by a single cutting tool will be generally quite easy to hold repeatable and a global note about inspection to the model will be easier than dozens or hundreds of dimensions. Fins on a heat sink or the position of cooling slots or holes are great examples of where not to specify dimensions. 5. Don’t specify unilateral tolerances. They are expensive to program and are more prone to causing scrap. Most shops will aim for the middle of a unilateral tolerance anyway so it won’t do much good to specify in the first place. 6. When applying diameter tolerances to chamfered holes, use a looser tolerance such as +-.010". The broader the included angle is, the harder it will be to hold the diameter tolerance at the top. A small Z change in the tool will result in a very large swing in size of the diameter. This is especially true of chamfers that are applied to a raw material face that is not finish machined. Because the surface to which the diameter relates to is not being established at the same time with a cutting tool, fluctuations in the diameter of the chamfer are very likely. 7. Don’t specify tight tolerance for the depth of a blind hole or blind threads. If you don’t want it to break out the far side, then specify that, but do not put a high depth tolerance. A minimum dimension and no breakthrough is probably the cheapest way to specify it. 8. Put information in as few places as possible. Don’t specify the material size both in the notes and as a dimension on a view. If you ever need to change it, you won’t forget to change both places.