Design for manufacturing (DFM) is a core methodology that ensures your die cast parts perform to specification and require the minimum of secondary operations. This is important when you consider that these operations can often represent as much as 80% of the component cost.
Download our on-demand webinar to hear our top tips for improving product efficiency, extended tool life, and lowering part cost.
Everybody welcome. Thanks for signing up for our webinar today on die cast design. I hope you have had the opportunity to attend one of our other seminars. If this is your first time we hope that you enjoy it. I’ve taken a screen shot of an example of the attendee interface just so that you know how to participate in today’s webinar. You’ll have the opportunity to submit text questions to today’s presenter by typing your questions into the question pane of the control panel. You may send your questions in at any time during the presentation. I’ll collect these and then we’ll address them at the end of the seminar to go over live for you. Also I’m recording this seminar today so I will send out the slides and video recording in the next day or so so that you can share with coworkers or follow up again if you’d like.
So with that I’d like to introduce Tim Sparkman. Tim is Dynacast’s premiere applications engineer. In June, so next month, he’ll have been with Dynacast for 25 years and is currently responsible for supporting the sales team with quoting and performing design for manufacturing on specific projects. Prior to this role Tim was the engineering manager at Portland and the Elgin facility for 18 years and the operations manager at Elgin for metal injection molding.
Tim has helped develop and launch hundreds of projects over dozens of applications from automotive, defense, electronic, consumer, and health over his career. Prior to working at Dynacast Tim worked as a manufacturing engineer at ITW, a quality engineer at Armstrong Tool, and was once a mold maker. Tim, thanks so much for presenting for us again today. You know, we had such great feedback from your die cast materials webinar, so thank you so much for taking the time for us.
Thank you, Taylor. Yes. I’d like to extend a warm welcome to everyone and again, thank you for joining our die cast design webinar.
I’d like to present the webinar from a tool designer’s perspective with an emphasis on design for manufacturing or DFM. As we go through the various design guide topics such as parting lines, ejector pins, gating and draft angles, I will explain what is generally needed for die casting in a manufacturing process, why it is important, and how these items may be illustrated on a part drawing.
Before we get into details I wanted to explain the typical Dynacast approach to launching a project. Dynacast will assign a project manager who may also be a tool designer. They will working with you on parting lines, gatings, critical features, ejector pins. It is very important that these items are discussed in the first few days of a launch while a tool is being designed.
The topics that we’re going to be talking about today will again be parting lines, wall thicknesses, draft angles, followed up by questions and answers at the conclusion of the presentation.
Die Cast Parting Lines
Okay. One of the first items we’re going to talk about is parting lines. One of the first things a designer needs to do however is to look at the requirements indicated on the part drawing. One key question that should always be asked, if the part design should be based on the 3D model or the 2D drawing. PPAPs and first articles are based on dimensions from the drawing, however 3D models being such a prominent design tool today, a designer can fall into sometimes a false sense that the model is the controlling document.
3D models are generally the design intent and after a design engineer reviews their stack tolerances of components and other critical features sometimes the drawing can be shifted as far as the tolerance zones. And again, it’s very important to have that dialog with the customer or at least interaction between you, the customer and us as a die caster to eliminate any headaches and grief as far as designing the tool against the 3D model or the 2D print.
As a designer reviews tolerances and critical features, Cpk values, and all data points on the drawing it’s important that they look at that from the tool design standpoint. Data points ideally should always be in the same half of the die steel which is normally the ejector half or the B half if you’re familiar with plastics.
As the part shrinks the ejector half of the die dimensions will become more stable. A designer should always try to lay out the parting lines or sometimes called mold splits to take advantage of these features. Having datums across various die components such as slides or the cover half of the die may create little variation which can affect tolerances and GDT result and possible secondary machining operations.
This illustration here shows a part that has a flat parting line. As you can see there’s a little bit of the radius that’s at the bottom which we would call this cover half of the tool, possibly the ejector half of the die here. An opportunity for possible cost savings is having a discussion on datums with respect to GDT and die layout. Moving datum points from one surface to another can sometimes improve the repeatability of a dimension on a part that is part of the DFM process. Advantages of not splitting a datum surface over two halves is dimensional layout and consistency.
If this surface here was your datum A plane, use this as an example, and let’s say this body diameter along here was your datum B or at least center point of this core pin. As you can see that this surface here, we would have datum A on one half of the tool and the majority of the cavity detail would be on the other half of the tool. If say datum B was the width and datum C for talking purposes was this core pin you would actually have a datum structure that would be two different parts of the tool. Again, datum A being the bottom surface here, datum B could be the width of the part, and say datum C for talking purposes could be this center core pin.
One of the advantages that we can do during a parting line is possibly split the parting line. We can take the parting line instead of having a straight jog coming right straight through the bottom of the parts is we could possibly raise the surface up through here, make this a compound parting line, skirt along this radius edge, and come through here. The advantage to this is during a measurement method is that you would have datum A, B, and C all in the same half of the tool making this surface here the ejection half and possibly the top here be the cover half or the A half if you’re familiar with plastics. The advantage to that is when you’re laying this part out let’s say on a CMM all your features and everything are going to be in one half of the tool and you’re not going to have split surfaces that may impact.
Sometimes on a 2D drawing engineers will identify this as possibly, if this was going to be your datum B surface, let’s say, you might have a surface that’s called B1, B2, and on the other side B3 and B4. What that would do is allow our quality engineers and your quality engineers to measure the part in the same location. And again, it’s important that the design engineer looks at this from your drawing standpoint so that when we go to measure these parts we’re not influenced by die mismatch or any other features that are created within the tool itself.
Parting lines don’t only control data points and dimensions. They can also have an impact on the life of the tool or component. Having a poor shut off on a feature will have an overall effect on the life of the tool, quality and product, and can also lead to production scheduling issues if the tool is constantly down for maintenance. This illustration shows a part that has two cored holes, one intersecting, and one intersecting at a 90 degree angle. Conceptually this is a straightforward, everyday type of situation we would run into.
I’d like to explain how this feature will be made in the die steel. On the right hand view here you can see that you have a solid main core body which would be your through hole here. You have a slide that would come in or possibly another feature, it doesn’t have to be a slide, it can be fixed in the tool and make this, the main body a slide. Then you’ve got a feather edge that is created by this round circumference here that would intersect the body to produce a cross channel through the holes. This feather edge is prone to wear and minor nicks around the edge due to the preloading of the core pin.
In die casting what we would do is we would actually have little preload on this core pin here, it may only be a half a thousandth to one thousandth of preload, but actually when this core pin comes in and actually is pressurized against this body, again, the body being this core pin here, we don’t want to have any flash along there so that this pressure or this surface here is completely seated along the mating.
This feather edge, again, is to be very prone to damage and wear. One option would be to modify this core by putting a flat. Now this creates a D-shaped hole that is shown in this illustration. However, we can make this two different ways. We can make this as a D-shape which would be adding a flat, or we could add a protrusion which would actually be adding a step so that if you did have a round shaft or a pin that was going through here we would actually take a small bite out creating an external flat on the part.
One of the advantages also by adding an external flat is let’s say this cross hole was going to be tapped for a set screw. When you tap a part there’s two different ways, we can either use a roll form or a cut form. Typically you have a roll form because the feeds and the pressures, it’s going to create a slight burr. If you want to have this full diameter here and a small little step here, again, this would be a step coming outward, it would allow a slight gap in the part so that any burr that is created by the roll form tap would be inside or at least outside the functional diameter of your pin to reduce any types of burrs that you might have on a part.
Parting lines on diameters. It’s always ideal to have an on a diameter anywhere from three to five thousandths of an inch flat that is shown and illustrated here. Some of the advantages of the parting line flats, it allows for any die mismatch not to impact the feature dimension. If you were to measure a diameter and if you actually measured on a 45 degree angle, the distance between this reading or the delta between this reading and the opposing 45 degree angle would actually tell you what your actual die mismatch is on a tool. Again, so adding a slight parting line flats, here we’re showing five thousandths, we can go as small as three thousandths on smaller parts. Again, it allows any type of die mismatch not to impede your functional diameters.
There’s also an advantage is that a lot of times what we’ll look at is gating along the surface or adding an overflow. By gaining or adding an overflow on a flat, vertical wall here it allows for a much cleaner gate break. If you were to try to gate along a tangency of a diameter here you’re going to have positive material, you’re going to end up having protrusions on the part. Again, a nice vertical wall allows for a clean gate break and also nicer just to gate in.
Parting lines on threads. In this illustration here it is also recommended that flats are added to threads, again, anywhere from three to five thousandths, and this depth is actually taken from the minor diameter of the thread itself. This helps to reduce any flash that would be at the root diameter or the V-sharp of the thread. Typically a die casting is going to be vibratory tumbled, possibly be thermal deburred to reduce any flash, but by allowing a flat alongside here it eliminates any type of minor flash, again, that you would have at the root diameter that possibly media, ceramic, plastic media would not easily get in between those nooks and crannies at the V-sharp thread.
On a small zinc die casting we also sometimes will gate along here or add overflows to help improve the flow of the thread itself. For those of you that were in our webinar for die casting about a month or so back, if you recall we had discussed eight velocities anywhere from a thousand to 16 hundred inches per second. As material flows in it wants to shoot by the crest of the threads and usually the threads become backfilled. So a lot of times what we’ll look at doing is adding a gate or overflows along the threads here to also help improve the fill.
Now obviously pipe threads we would not add parting line threads. Pipe threads typically would be thermal deburred as a secondary operation to reduce any kind of minor flash that you would have, again, along the root diameter.
So in conclusion on the topic of parting lines, I hope you understand that there are many things to consider in the parting line jogs of a part. These items should be reviewed and not taken lightly. Parting lines or mold splits should also be shared with your team as well. If the part is intended to be used in a feeder hold,our parting line is going to have a major effect on how the part assembles or engages in your manufacturing process. Typically a GoToMeeting is offered so all parties can review the part layout and understand critical features.
Besides parting lines gating is the next important item to navigate. For those of you that attended, again, our die cast seminar, we again talked about the high surface speeds that material travels at, we also talked about, you know, fill times, anywhere from 15 to 40 milliseconds depending on the size of a part. Metal pressures can be anywhere from three to four and a half tons per square inch.
Like parting lines there can be several options when we’re looking at how to fill a die casting. Some of the things a designer will look at is the shorter distance of travel. Both zinc and aluminum cool very rapidly and they can be…and what you want to do is look at the gate for the shortest distance so a material will not cool as fast which also helps improve a better sounding casting.
Now in this area here we’re showing an in gate or an edge gate along the part here, but it’s going to have to go the length of the travel. Now again, this is just an illustration, there might be reasons, you know, that we could have possibly gated along the side of the part which would give you the shorter distance, you could have had a gate that had a fan that would have helped fill this area in here, and also flow in this area through here. But again, this part here is laid out as an edge gate that will allow the material to flow down the part.
Now one thing for those of you that are in plastics, you do not typically see a knit line or you won’t see a knit line on a die casting as you would in the plastic part. Because we atomize our material because of the high gate velocities that we have and the way the part actually fills you do not see a wave front that comes through. That’s not to say that we don’t have areas where the material flows in a little bit slower, but that we can actually do through mold flow which I will show you in a moment here.
Other things that we can look at from a gating standpoint is areas to fill the part, and again, this is something that’s done during the DFM process. This is actually a customer’s part that we did and one of the things that we had to concern ourselves with is fill into this bottom post. Any time that you’re filling in a cavity detail that’s what we would say the blind piece of steel, meaning that the parting line is going to skirt alongside this edge and this bottom post is going to be a blind piece of steel, there’s no slides, it’s very difficult to add any venting to this post so that we can improve the fill of the part. By adding this so-called gusset along the part, this allowed us to add a gate where we could favor this pin. We also add a divot on the part here as a cone, so as the material flows in rather than it just shooting straight by this post this divot acts as a diverter and helps to drive material down into the post.
Now some of you might be thinking, well, why don’t you just add an ejector pin at the base of the post? Well, the part we would…so again, this is the original concept, this is what we came back in and offered to the customer for fill. One thing that is sometimes difficult on the die casting to fill is blind features, and again, this post would be in a blind…the parting line would skirt along this edge, this post would be blind.
One thing that most of you might be looking at and saying, well, why don’t we just put an ejector pin at the base of this pin, and we can and we would for ejection purposes, but one thing I’d like to say is that at times it’s trying to evacuate a 55 gallon drum of air with a straw in about 15 to 20 milliseconds. Are we going to get some air through there? Absolutely. But is it going to be enough to have good, strong integrity on that post? Again, adding a diverter here is something that can help improve.
Mold Flow Simulation
One of the tools that Dynacast has is our mold flow simulation. This is illustrating how the material actually fills into the part. This has a blind and it also has a shaft. On the shaft here a bearing was going to ride and the customer did not want to have any parting line along this, plus this blind detail itself would create an undercut that had to be made in a solid piece of steel. As this thing illustrates, you can see the material kind of flows and really favors that shaft portion, and then it backfills into the body of the part. So again, you can see the material fills into the post, it starts to backfill onto the body, as it fills and pressurizes the back cavity the material starts to move forward where we have a parting line and actually then it starts to fill in our overflows which are later vibratory degated off the parts so that we have a very good, sound structural casting.
Again, we can run a multiple simulation on concepts. So if you have a 3D model that’s just conceptual our designers can go into sketcher mode, we can kind of look at a couple of different gating proposals, run the simulation, and actually see if there’s any shortcomings, if there’s any features that we may want to possibly make a suggestion as diverters or something to help our material flow into the part a little bit.
Weight savers. As just mentioned on the design it’s an idea…when we’re talking about uniform wall thicknesses actually from a filling standpoint, you having a uniform wall thickness is very important. Weight savers not only save cost and material but we can also improve cycle speeds which helps reduce the part cost, not just in raw material but also faster in processing.
Adding Ribs to Die Cast Parts
Some of the weight savers could actually be modified into ribs. These ribs can have several benefits. The ribs can act as a fill channel. Say you have this center hub area here, if we needed to allow material to flow, you know more into this we can favor our gate so that we can actually have our material flow into this hub for better fill within that area.
Also take advantage of ribs. As you can see these have some ejector pin bosses are in the outside of the part. I mentioned earlier that a lot of times die castings are vibratory tumbled, either plastic, ceramic, or steel, sometimes even shot blasted. If you have an ejector pin at the base of a part a lot of times, especially with media it acts like a cup. One of the advantages of doing the vibratory tumbling is the, by say ceramic or plastic, is the agitation and movement of that media across the part helps to reduce any sharp edges or any minor flash that you might have within a part. When it’s recessed into a deep pocket the media tends to collect there and basically will sit there and it doesn’t have a chance to agitate. As you can see, by adding the ribs it allows the ejector pin to be on the outside surface which will easily be attacked by the media, circulation of the media.
Another advantage is structural strength. You can actually add some ribs in here to help not only to fill the part but also give it some structural strength within the part itself.
Here’s some suggestions basically from kind of a before and after. If you have a solid part, and again, a lot of times where die castings come into play is the opportunity comes in for a machine part to do a die casting. A lot of these examples could be typical screwing machine parts of machine billets that you’re working on today to come back in and pour out all this detail maybe on a part would be very costly from a secondary standpoint. However, from a die casting standpoint it’s very easily and also preferred from that standpoint.
So as you’re seeing this area in through here, you know you can add a weight saver in the part, and again, trying to take advantage of uniform cross sectional area, and let’s say from the side view you can actually see some strength that’s in here. A lot of times the strength of a die casting actually is formed by the skin of the casting, and that skin can be a couple of thousandths up to say 20 thousandths of an inch, is really where you get the strength. So having a massive cross sectional area in here really just adds weight, it doesn’t give the part an improved mechanical advantage from a strength standpoint. And actually it would…actually you would end up having a higher probability of having some porosity within the part just because of the thicker cross section.
And again, if you have a screw machine part of some sort that you that you do It around you might be able to come back into a hub area here adding some cost or some cost reductions to the part as weight savers, and again, kind of like an angle block here that you’d have just adds some feature to the part from that perspective.
Fillets and Radiis
Fillets and radiis and we’ll also throw some gussets in there. Not only do these features help material flow and how the casting will fill, but it also improves strength and helps to reduce any stress risers within the part. Again, when we talked before about that post that we added a diverter in, again, when material is going as fast as the velocities that we’re looking at in die casting, again, a thousand to 16 hundred inches per second, material does not like to do a lot of 90 degree turns. By adding some radiuses and some fillets into a part it helps dramatically improve the fill characteristics of the part.
Radii and corner breaks can also reduce any types of nicks during shipping. A lot of times parts, die castings are shipped in bulk process, usually cardboard box. So having nice, generous radiuses on a part helps reduce any types of nicks, handling damage that you might have, and also from an operator safety standpoint any sharp corners and edges that you have within a part itself, make the improvement.
Draft is a big question and it usually comes up as probably one of the biggest topics usually of any type of seminar that we perform. Unfortunately there is no set answer and this depends on several factors. Our design engineers will work with any of these features, however, to give you some indication as to a die caster’s perspective, and what does draft angle actually mean to us. On top four topics that are usually an item to look at, wall thickness, the length of the feature or the distance, parting line layout, and ejector pins.
One thing to keep in mind is the part shrinks, it will always shrink to the center of gravity. For those of you that are in the 3D CAD files, usually if you hit your mechanical properties or properties you can actually see where the CG point is, and again, this is where the die casting is going to want to shrink to.
Wall thickness, you know, having a uniform wall thickness within a part by adding weight savers can have several advantages. It allows the part to cool uniformly, it helps to reduce any type of weight that you might have in a part, but a lot of times die castings are pushed to become thinner wall sections, usually for weight reduction.
So let’s use an example. If we had an aluminum housing, and let’s assume that the wall thickness was two millimeters or 80 thousandths, and the height of the housing was say three and a half inches or approximately 89 millimeters. If there were no ribs on the sidewalls of the part, if you looked at where we added ribs before and we showed the ejector pins on the part, previous slide, let me just jump back here a couple of slides here just to show you, if we had a large deep pocket, and these ejector pins were at the base of the housing, and you had a very thin-walled part, we’re going to have to worry about or look at distortion within the part itself. Without having any ribs on the part we would have to have large ejector pins on the surface of the part. The large ejection helps to ensure that the pins don’t push through the part or dimple the surface.
The sidewalls of the housing could be drafted anywhere from one and a half to three degrees per side allowing the housing to properly eject without warping. Draft is as much a function of the tooling as process is to the design engineer and the products engineer which need to work closely. So again, on wall thicknesses where it’s important is on very thin walled parts we need to look at how much draft angles we can actually have, where the ejection is on the part. If we don’t have adequate ejection then we need to have a little bit thicker wall section. So again, they kind of go hand in hand.
The other one is length versus distance. Castings will shrink anywhere from six to seven thousandths per inch. On small parts this may not be a huge factor, however in a large casting where the span could be several inches the part could have shrink rates exceed a 32nd of an inch or even more between the features. When there isn’t adequate draft on a feature such as a core pin used to produce, let’s say a hole, the result can be the hole becomes elongated or in worst case, the core pin breaks due to excessive amount of shrink.
This also is why sometimes, a lot of times on die casting we’ll make self-tapping holes on a part, on a very large, again, several inch span of a part to do a self-tapping screw. Usually the self-tap manufacturers will allow very, very minimal amount of draft on the hole, and again, when you have shrink factors that could be diagonally on a large part that are exceeding 30 or 40 thousandths of an inch, that’s a tremendous amount of shrink and on a small pin, let’s say three millimeters in size for a self-tapping screw, you’re going to have two situations. Either those cores are going to snap or possibly the hole is going to be elongated which is going to affect your engagement of thread.
So again, understanding the challenges of a die caster because of the shrink factors that we have, you know, draft angles are very important so that we can actually maintain the tool, that the part comes out straight and perpendicular to the ejector side o the tool.
Outside surfaces on the housing, let’s say again because the part is shrinking inward, can be anywhere from a half to maybe one degree on the external side.
Parting lines. Parting lines typically don’t have a major impact because again, parts are shrinking inward, but if you have slides, slides are going to require some amount of draft such as cored holes that you might have on a part.
A lot of times on a drawing customers will refer to draft within tolerance, but again, knowing that you have excessive amount of shrinkage, again, six to seven thousandths per inch, sometimes what we’ll look at doing is adding a kind of a stepped draft angle into the part. Instead of just drafting within tolerance if you have a hole, especially if you’re doing any type of secondary insertions of the shaft or pin or something to that effect, what we can do from a die casting standpoint is give you a half degree draft lead in, shorten that draft, and then say the maybe two thirds of the distance draft within tolerance or maybe even take a third of that detail and draft zero draft.
One of the advantages of drafting on a core pin like that is that if you’re inserting something in there it’s easier for an operator or a machine to insert a component, allow the part to be seated, and then you can do either your crossfit or however you’re assembling your component.
And I mentioned ejector pin layout, it’s very important that we have adequate areas to eject the parts so that whatever draft angles we have either have significant adequate draft or minimal draft. If there’s minimal draft angles on the part then we definitely have to rely on good solid ejection pins to push out the part. And again, if you have a very thin-walled section with very little draft we have to go with big ejector pins to get good surface area to push out on the part. If not the ejector pins either A, push through the surface or a part, or dimple it which could impact flatness on a part as well.
Flow. Improvements for flow. Again, mentioned before, material doesn’t like to do 90 degree bends. So if you were to gate along this surface here and we had this window material would have to shoot around here and come around. So you can just see there are some features, again, these are things we can work with you to help make improvements.
So manufacturing techniques here that you have, again, D-shaped holes, something that we can cast, again, this is taking advantage of the die casting process possibly opposed to secondary machining if you’re doing a screw machine part. Adding these types of features may add additional cost, and it’s also value added. Rather than doing two pieces we can combine two or three parts possibly. In this case here you’ve got knurl with a shaft and we’re showing here that we can make this as a one piece die casting.
Holes in slots, we can add jogged parting lines here, but if possible, if we could avoid this helps reduce some of the costs tooling wise. You know, if you have holes that are coming in at different angles it’s not to say we can’t do this, but this is definitely going to impact the cost of the parts. Again, we try to keep the features in the open and closed draw which is indicated by the arrows of the part
Knurls, logos, those types of things, again, this is kind of straightforward. One opportunity to at least keep aware of is any type of tick marks or any type of outside markings that might help aid your operator or possibly robot from a vision system, you know, take advantage of the die casting. If we can add some type of features, again, if we can make it easier for the operator to see that the part needs to be orientated or something to that effect.
We can do surface textures as far as a light EDM surface, you know, to help make the part look more esthetically pleasing which would be a matte appearance.
So in conclusion to our die cast design webinar, I hope that everyone was able to take away a little better understanding of the die casting world of manufacturing, how parting lines are not just a foundation of a good tool design but how split lines can have a direct impact on the quality, measurement, and performance of a product, how draft angles are influenced by several characteristics of die casting, and stating a simple, one degree draft angle isn’t always a one size fits all.
We encourage you to reach out to us in early design concepts. We may be able to offer cost savings to help you in your design, help explore value added by consolidating other components or other features into your product to help further reduce your cost.
Thank you and I will turn this back to Taylor for some open questions. Thank you.