I have been working on CADing a few chassis, and I was wondering how do people actually make the diamond extrusions in the CAD. I cannot find a way to do it that doesnt take hours of work, and I am sure there is a better way.
You should use a sketch pattern. If you are using SolidWorks, when making the sketch, after you draw a diamond click the linear pattern button under the sketch tab. From there you just have to tell it what directions and how many patterns in those directions.
Inventor is very similar.
Both SolidWorks and Inventor should tutorials online on how to do this.
-Nick
What CAD software are you using? If it is SolidWorks then I can send you CAD files with some examples of the type of base plate you are trying to make.
If you are using inventor I can send you a step file, but that doesn’t provide any insight into the design process.
Edit: Should Have Seen this was posted in the inventor section. My bad.
A lot of programs allow you to create features using rules. What I have done in the past is define a series of points where I want the lightening features and then have the computer follow the rule that places those extrusions at those points. It takes for ever to set up, but you only really have to do it once.
Depending on the program you use, the names for this might be different. For inventor it is all done under I-Properties.
Here is a dull demo for inventor 2011 
Proper instruction videos are also available on youtube.
Good luck 
I tried doing that, but how do you get it so it perfectly fits the width and height of the plate. It always ends up that they do not line up correctly in the end.
I have been using inventor for a while and have done some diamond plated baseboard.I first create the diamond sketch on the plane then choose what type of an array I want.Then generally use rectangular array and select the dimension and how many i want in each row and column.Then I extrude them and the filet the tops
- Draw center lines for the center of all of your ribs, and tweak the geometry as needed to make sure all of the ribs look good.
- Convert all center lines to construction sketches.
- Select all of these construction lines and use the offset line tool to offset them.
- Use the power trim tool to remove all unnecessary line segments.
- Extrude cut the holes.
- Use feature fillets to add fillets to all of the corners. I almost never use sketch fillets, as they can be difficult to remove / edit later on.
Just to add another method (that I think will work) you can also make the appropriate ranges using linear pattern in sketch, and then extrude the triangles. In the Extrude menu check “Draft Inward” and make the degree very steep, to get the diamond plate effect. I also think that you can extrude all of your diamonds in one extrude command, and thus later change the drafting angle and the overall look of the diamonds pretty easily.
Hope that helps!!
It took me about 6 tries over 4 hours to get it right. Don’t think that those of who are coming up with this sort of work are insanely skilled or have some magical way of doing this quickly. It really takes a lot of time.
It took me about that long just to fillet all the corners. There were like 300. I’m not sure that was worth the effort.
Did you use filletexpert?
Also, you can fillet before the pattern.
Yeah, I’m with you on that one. My CAM software would have just done toolpaths that would have given me a fillet radius of the tool radius, but I don’t want the tool to squeak in the corners when milling, so I put in all the fillets. I could pattern many of them, but after adding all the electronics mounting locations, there were many that had to be manually put in. It takes a decent computer. And for all you who waterjet your diamond pattern baseplates, yeah, we did ours on a router. 6 hours of babysitting a machine with a spray bottle of WD-40 in-hand. In the end though, I’d say it was worth it. If done well, it’s a really nice piece, and makes it a joy to weld and wire.
I figured out a way in Solidworks that reduces it from a tedious process to a single feature and 2 mirrors (really speeds it up because it eliminates the patterns and associated lag). To do this I draw out the belly pan in 3 steps. Step 1 uses extrude thin, step 2 and 3 use mirrors about the front and right planes.
If I were to do this in Inventor I would do a similar process but instead of using extrude thin (drawing just lines) I would actually draw out the first shape.
In all this process takes the hours long drawing and turns it into about 10-20 minutes. At least for me this has almost no lag, this is likely because the process reduces the number of relations (what slows the model down when patterning).
My poor old little laptop dies when I try those patterns -__- I need a new laptop. I end up suppressing them while working on stuff anyway.
It was more because of all the extra mounting geometry we added in.
I was using Inventor at the time, and if an equivalent Filletexpert exists, I didn’t use it. I still haven’t learned how to use it, but now I might look into it.
Yeah, we didn’t want the sharp corners from the laser or the extra time it takes when the machine doesn’t smoothly run through the corner. The time and machine wear considerations weren’t really for us so much as they were for our sponsor.
But hey, at least you have a nice big router. I can think of at least a few (hundred) uses for that.
Getting the pattern to line up with the ends of the plate just takes some trial and error (or math, if you’re clever about it ;)). I create a test version of the pattern in a sketch to check this because it’s faster for me.
I’ve found a way using patterns, mirrors, etc. to do it fairly efficiently. The part’s rebuild times are bad (up to 40s on my computer), but full rebuilds are rare, it is otherwise fast, and produces exactly what I want, not some representation.
Here’s how I do it:
- Create a sketch of one corner of the baseplate - two triangles and two square/rhombi
- Extrude/Cut each shape and add fillet features individually
- Make a pattern for each shape: one triangle along x axis, the other triangle along the y axis, the rhombi along the x and y axes. The rhombi must be patterned separately, as the number of them along the x and y axes is different for each one.
- Mirror the triangle patterns across appropriate planes
- Add extra material and holes for gearbox cutouts, electronics, etc.
This process is illustrated in the attached images. Feel free to ask if you have any additional questions!
Try using the fill pattern feature in Solidworks 2012. Google for YouTube tutorials.
Should take less than 5 minutes to generate the pattern
Create the base plate
draw a line for direction of fill
select full preview
enter boundry margin
create a seed cut, select diamond at 45 deg
select a seed pattern
select spacing
