October 19, 2012
Columnist Gerald Davis is ready to rip into the process of converting imported 3-D parts to flattened parts.
Consider a scenario in which a CAD model has been imported as a dumb solid model that lacks any feature history. Such models require slightly different editing techniques from a fully parametric model. This is a common occurrence with downloaded CAD models. In situations where you need to manufacture the item represented exactly in the imported model, you may not need to take further action. If the model is incorrect, however, you obviously will need to correct it before sending it on to fabrication.
In the case of an imported sheet metal model, the main issue is compatibility with your available forming tooling. Tooling selection will have an impact on the ideal flat layout calculation. Editing will be required in order to get the dumb solid to unfold into an automatic flat pattern.
Our mission in this article is to get the model shown in Figure 1 to unfold so we have an automatic flat pattern. We are going to compare a couple of methods for accomplishing this. The first technique we consider uses the inside bend radius found in the imported CAD model. The second technique gives us the ability to change the modeled inside radius in our version of the product.
(Please note that although this column mentions a brand of software by name, the general topic is sheet metal modeling. To that extent, the article may be relevant to fabricators using other CAD systems as well.)
As SolidWorks® looks at the model in Figure 1, it almost sees sheet metal; the wall thickness is uniform throughout the model. The problem is that this model cannot be made on a press brake. The seams that allow the corners and flanges to fold from flat stock are not there. This part would have to be machined, cast, or magically stamped.
To help SolidWorks unfold this, we need to rip some gaps into the model. From there SolidWorks can do the rest of the flat layout work for us.
In this example, I’ve opted to make a 90-degree kerf cut pattern. You might prefer to use a 45-degree mitered corner, or rip the part in some other way. The modeling goal is to have a bend relief anywhere that two bends intersect each other. Basically, the part has to unfold without tearing.
I’m slightly abusing the term ripping. SolidWorks has a tool—q.v. Rip—made specifically for ripping of sheet metal. Ripping is also a part of the Convert-to-Sheet Metal tool. Those tools take unique advantage of sketches and features and are more suitable for other kinds of models. Our imported CAD in the example shown in Figure 1 requires special treatment. The modeling we are doing would more accurately be described as cut-extruding than ripping. Our goal is the same as with the ripping tools: to separate flanges that would otherwise require stretchy metal in order to unfold.
Figure 2a shows a first step in our ripping process. We cut away the corners so the part resembles sheet metal before welding. I made that cut by sketching four squares on an end surface of the chassis. Their outer corners intersect with the outside of the flanges. Their inner corners lie tangent to the outside of the bend radius.
We have not dimensioned the material thickness or the bend radius yet. We are relying on—and relating our sketches to—the as-imported model so far. One little trick I pulled was to run the cut past the flange to prepare for the kerf cut’s separation of the vertical from the horizontal flanges. In this example, I offset the corner cuts 0.030 in. past the face of the flange. This is what I’m allowing for springback when forming this part. Note that the extra cut length just cuts empty space for the upper two corners. The offset is meaningful only where the cut passes into the horizontal side flanges.
Figure 2b repeats the process from Figure 2a. To make this cut, I used a derived sketch based on the sketch from Figure 2a. This saves a bit of sketching time. To create a derived sketch, you select the sketch you want to duplicate and also the surface you want the duplicate to be on. Then use the Insert>Derived Sketch command to drop the sketch in place. You may need to add a constraint to locate and fully define the derived sketch. As with the first cut, this cut is offset past the flange by a springback distance.
Figure 2c finishes up our ripping cuts by separating the vertical flanges from the horizontal ones. This is made using a sketch on a plane that lies inside the chassis, which makes it easy to cut through all in both directions. In this example, the plane on the right side is shown. The sketch is simply two rectangles with sketch relations to our previous cut features in the model.
If you compare Figure 2d to Figure 1, you’ll note that the ripped model is faithful to the original except for emerging compatibility with fabrication. We now can let SolidWorks recognize this model as a sheet metal part. How we do that will determine how much control we have over the subsequent inside bend radius.
The Sheet Metal toolbar has an Insert Bends icon as shown in Figure 3a. That icon launches the Insert Bends Property Manager shown in Figure 3b. I rotate the model to make it easier to select the face I desire as the fixed face. As the part unfolds, the other flanges move to unfold around the fixed face. The system recognizes the inside bend radius and thickness. We can change the K-factor—or select a different layout method. Click the green check mark to dismiss the Insert Bends Property Manager.
We now can flatten the sheet metal model by clicking on the Flatten icon in the Sheet Metal toolbar (see Figure 3c).
Figure 4 shows a 2-D fabrication drawing for our ripped sheet metal part that features inserted bends. The bend table is related to the flat pattern layout shown on the right. That layout has letter symbols adjacent to each bend. The table makes a tidy presentation of bend direction, angle, and radius.
To check the work, if I were laying this out by hand, I’d use a 0.104 bend deduction for 0.063-in. aluminum with a 0.062-in. radius; 11.784 would be my layout. The K-factor I used in Figure 3b—0.4857—appears to be pretty close, but 0.4840 would have been better.
You can adjust the K-factor to get the flat layout you need to match your tooling. That does not change the modeled bend radius, however. If for some reason you require a model that allows you to edit the bend radius, then Convert to Sheet Metal is more fun.
Looking ahead a little bit, Figure 5 is similar to Figure 4 but shows a model with an inside bend radius of 0.047 in. The original import had a radius of 0.063 in. The entries in the bend table show the radius rounded to 0.05 in. But, I got ahead of myself. To produce this drawing, we start with the just-ripped model shown in Figure 2d.
The Convert-to-Sheet Metal tool will attempt to honor the existing bend radius, just as Insert Bends does. To avoid this, we are going to delete the modeled bends before launching the Convert-to-Sheet Metal tool. I will demonstrate the face deletes in three steps. Note the option setting for Delete and Patch in the next series of figures.
Figure 6a shows the selection of the outer bent surfaces as well as the inner bent surfaces. If I try to select too many intersecting surfaces, the preview will fail. I have a personal habit of trying to minimize the number of entries in the Feature Manager’s history list. That is the only reason I combined the selection of faces for Delete and Patch the way I did. You may find another method of removing the modeled bends to be more convenient. If you do, please let me know.
Figure 6b shows the similar operation repeated for the other end’s bends. It also shows the results from Figure 6a—the smooth bends have turned into sharp edges.
Figure 6c shows the selection and deletion of the fillets for the remaining bends. With all of the modeled bends removed, we now can launch the Convert tool as shown in Figure 6d. I flipped the model over to make it easier to select the fixed face that I desired. It is highlighted with a blue border. The system discovered the thickness—0.062 in.—for me. I entered the value 0.047 in. for the inside bend radius. That matches my tooling. I then went around and selected the outside edges that I want to turn into bends. Those are shown with pink selection highlighting.
The converted part is shown in Figure 7. It looks a lot like Figure 2d, except for the bend radius. And we can change the inside radius by editing either the Convert-Solid feature or the Sheet-Metal feature. Figure 8a shows the editing process for the Sheet-Metal feature. I’ve changed the radius from 0.047 to 0.032. You might also notice that I’m using the Gauge Table option. This is a good way to standardize the bend radii and K-factors that get used.
Figure 8b shows that the 2-D fabrication drawing updates to show the new inside bend radius and flat layout size.
Please keep in mind that you can use several methods to rip a sheet metal part so that it will unfold. There’s also more than one way to insert a sheet metal feature to get a part to unfold. If you need to edit the inside bend radius, delete the modeled bends before converting the part to sheet metal.
Gerald would love to have you send him your comments and questions. You are not alone, and the problems you face often are shared by others. Share the grief, and perhaps we will all share in the joy of finding answers. Please send your questions and comments to email@example.com.
The FABRICATOR® is North America's leading magazine for the metal forming and fabricating industry. The magazine delivers the news, technical articles, and case histories that enable fabricators to do their jobs more efficiently. The FABRICATOR has served the industry since 1971. Print subscriptions are free to qualified persons in North America involved in metal forming and fabricating.