A single assembly may not serve well for all purposes
June 13, 2012
Columnist Gerald Davis focuses on creating better illustrations and models to make life easier for parties involved in downstream operations.
Figure 1 shows a lift table lying on its side to reveal the crank assembly. This sort of illustration might be useful in a brochure or for design review. Figure 2 shows the same table in a more normal orientation. The goal behind those two images is to give the casual observer a sense of the product’s capability and finish. These computer-generated images feature shadows to help add credibility to the illustration.
Figure 3 is an attempt to indicate that this lift has a functional upper limit. When extended to an excessive lift height, the lift can tip over from just the weight of the tabletop. With safety issues in mind, a fabricator might find Figure 4 a little worrisome because no wheel locks are evident. Or perhaps Figure 4 shows the merits of the table as a piece of exercise equipment.
All four of these illustrations have something in common: the use of a familiar object to give scale and lend focus to the product. They also use lighting to give suggestions of color, texture, and material. A variety of “bling” items—coin, soda can, and mannequin CAD models, for instance—are readily available online.
When modeling for illustrations like these, you can set aside considerations about the bill of materials (BOM) unless, of course, the scenery items need to be included in the BOM. To create this type of illustration, drop your manufacturing assembly into a studio assembly. Use that studio assembly to add the setting and scenery pieces in that playground context without disrupting the subassembly that represents the model dedicated to manufacturing.
While the studio assembly is not usually intended for general distribution—because its entire purpose is for generation of animations and still shots—it is still an important part of the CAD database in that it can be retrieved and edited in the future. As wonderful as Figure 4 might be, it could be improved upon—perhaps by you.
When creating these graphic items, you need to keep your models well organized with good file names and folder layouts, clear descriptions in the models, and plenty of comments to explain the existence of illustration elements. To illustrate the importance of naming and comments in your CAD data, consider the process of creating a video to show the lift mechanism in motion. We will need configurations, a distance mate, a motion study name, and a movie name.
This next bit is very specific to SolidWorks®, the modeling software that I use. The purpose of the dedicated configuration of the lift table is to allow a distance mate to set the elevation of the tabletop. A separate configuration of the lift table will suppress this fixed distance mate and replace it with a limit mate. That configuration will be used when animating the mechanism by mouse drags.
With the configuration with the fixed distance mate active, a motion study can then be created to vary the distance mate for the table elevation from a minimum to maximum value over time—say, from 6 to 20 inches starting at one second and ending in 10 seconds.
Included in our mate scheme in this lift table assembly is a gear mate between the ACME lead screw and its bearing nut. Because of the chain of mates, as the table elevation changes, the ACME screw and crank have to turn.
Since we are clear on what our configurations’ purpose is, inventing meaningful names is easier. We’ll create a configuration named For Motion Study 1. The description comment might read “Distance Mate1 is active to set the tabletop elevation.” The other configuration might be named For Live Demo and described as “Mouse drag tabletop between 4 and 20 inches.”
We are using this lift table assembly model for several purposes—illustrations, animations, and fabrication. As an exercise, we are going to start manufacturing documentation for the assembly shown in Figure 5. In this scenario, our customer has thrown this over the wall to us for fabrication.
The Feature Manager to the left of the graphics window in Figure 5 shows the current file names of the components—quite a variety of common names and part numbers. The model in the graphics window looks to have a functional design, but reflects the final stages of design exploration. The modeling techniques are the result of efforts to visualize rather than efforts to optimize for revision management or rebuild time. And we note in Figure 5 that the BOM information is missing part numbers, material, and source for all items. The descriptions don’t seem to be any too tidy, either.
It is our responsibility to manufacture tables that strongly resemble this model. Those gifting us this mess have acknowledged that they were going for look and function more than manufacturability and specific dimension.
We need to proceed with minimal impact on function. Nonetheless, we have full responsibility and authority to have our way with this CAD database. As we edit the CAD model, we keep our main deliverable goal in mind: Fabricate a crank-driven lift table that lowers below 6 in. and lifts above 22 in. We intend to lift a 75-lb. box that is 19 by 19 by 19 in. In a more realistic scenario, the design specification would include caster footprint, shipping weight, assembly skill, finishes, cost, and so forth.
In addition to validating the design of the mechanism, we have several deliverables to produce. The manufacturing shop requires fabrication drawings for sheet metal, weldments, and machined parts.
COTS is an acronym for “common off-the-shelf” and refers to commodity items like nuts, bolts, and wheels. Purchasing will need to know all about COTS items as well as all raw material and subcontracting requirements.
Shipping will be looking for packaging details—a set of cardboard items, product kitting assembly, labeling, etc. The end user will want to have useful assembly instructions. By focusing on documenting and validating the design at the component level, the CAD operator will find that the other deliverable documents will be largely a matter of selecting the appropriate template.
For each component, we need to assign part numbers and descriptions and to identify sources for each item. Along the way, we’ll tidy up the file names and CAD modeling techniques.
I believe that our first step would be to make a working copy of the model that was tossed over the wall to us. We don’t want to burn bridges. We will treat the original as the master quality control document. Our copy will be the only one we edit.
You might already be aware that file names in a CAD database come with strings attached. Changing the name of a file can have undesirable consequences. For example, two files are required for a drawing of a tabletop—a 3-D model and a 2-D drawing file. Within the drawing file is information that includes the file name and last known location of the 3-D model that it needs for its projected views. If either the file name or location is bogus, then the drawing will not display correctly. As a result, the CAD software includes tools and procedures for changing file names in a coordinated manner to preserve the external links between drawings and components.
As an example of why we might want to change the name of a CAD file, the model we are starting with uses common language in the file names—for example, ACME NUT BRACKET.sldprt. As a job shop, we might have a dozen customers that we manufacture ACME nut brackets for. As long as they are kept in their proper project folder, the CAD operator should have no problem keeping the jobs organized.
However, as this project moves through manufacturing, marketing, purchasing, and other departments, the file will appear in multiple folders. To minimize confusion caused by duplicate file names, our shop has a policy. We use the part number as the file name. We can do that safely because we assign a part number only once; two different items will never have the same part number and revision. Information like description and revision will be kept in the file properties of the CAD file. Fortunately, in this scenario only six files need to be renamed and 10 others already have part numbers for COTS items.
Figure 6 is a screen shot of a Pack and Go dialog. A column in the table lists the Save To Name. The entries in green are the files that I have renamed. Each brand of CAD software has similar tools for changing file names. I’m fond of working with this tool because I can see all of the file names and paths in a convenient list. It has a very handy Select/Replace button to speed the renaming process.
After we make a copy of the master assembly, we close it without saving anything. We may never open the master file again. We switch to the new folder location with our fresh copy open in it.
Figure 7a shows the working copy of the assembly. You might be able to see that the file names in the Feature Manager’s list are looking good. While the file names are correct, I notice that the components appear in no particular order. As a matter of policy, our shop likes to have custom-fabricated components at the top of the list, followed by COTS items.
To rearrange items in the Feature Manager, just click and drag. Here is a time saver: If you preselect several components—use the CTRL key while clicking—you can drag them all to appear in sequence wherever you let go.
The cursor will change to show you the destination of the drag. Not only can you rearrange things, you also can drag components from one subassembly to another. We don’t want to change the subassembly, so we will hold down the ALT key while dragging to prevent subassembly shuffle. The cursor will be a little yellow arrow to show that we are just rearranging.
Figure 7b shows the result of a few moments of dragging. All of the custom-fabricated items are at the top of the list. This is the default order in which they would appear in a BOM table, by the way. I left the custom-fabricated items highlighted to make it more obvious that they are at the top of the list. While this rearrangement is not essential, I find it is useful as a method of organizing and planning the work to be done.
As recommended in previous episodes of Precision Matters, our shop has used the Property Tab Builder to design a data entry form that is coordinated with our template for BOM tables and with our template for drawings. With our assembly open, we now use that data entry form to type in the data for descriptions, materials, and finishes.
In Figure 8a, progress has been started on the third component. It is shown as selected in the Feature Manager’s list to the left of the graphics window. The Custom Properties data entry form appears to the right of the graphics window. I’ve inserted a BOM table into the assembly so I can quickly see errors and omissions. Figure 8b shows the result of a few minutes of selecting components and typing. We now have a complete and accurate BOM table for our top-level assembly. File names and descriptions are now correct.
The next stage in our work flow is to produce manufacturing drawings. Let’s start with item No. 4—the bracket for the ACME nut. It is shown open in its own window in Figure 9a.
Figure 9b shows the result of selecting a drawing template to use with our 3-D sheet metal model. Note the isometric view and the three orthogonal projections to the drawing arrive without dimensions. The better news is that the title block and all notes are automatically completed because of the previous data entry labor.
Figure 9c includes dimensions after a little bit more labor. Some of these are imported directly from the model. When needed, we added dimensions to fully detail each view according to our drafting standards.
For some items, we might want to include a flat layout on the drawing. To do that, we could add a sheet to the drawing and then insert a view of the flat pattern as shown in Figure 9d. I added overall dimensions to help with the cost estimating. The system automatically inserted the notes that indicate the bend radius and bend direction.
If we need to generate a DXF file for CNC programming, we open the sheet metal part and right-click the mouse on Flatpattern1 and then select Export to DXF/DWG. A screen shot of this is shown in Figure 10. From there we give it a file name and perform entity cleanup so the DXF arrives at the destination ready to go.
Please keep in mind that the mechanical drawings will be needed for all of the custom-fabricated components in the lift table. This article discusses making a drawing for only one of the parts. The drafting process would be repeated for the tabletop, scissor legs, and axle hubs.
Next month we’ll continue our theme of speeding the manipulation of CAD models for the benefit of manufacturing.
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 firstname.lastname@example.org.