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Lower suspension attachment clevis assembly drawing

It seems that other people who’ve built cars from scratch attempt to get their cars rolling on the ground as soon as possible, so I figure I’ll do it that way too. With that in mind, it’s time to start fabricating the suspension. First up: lower suspension attachment clevises. I ordered 7075 aircraft aluminum from the United States as part of my big shipment. It’s amazing stuff– stronger than steel but light as aluminum. These assemblies have to be extremely strong, as I calculate that under braking the front one takes a load of over 4400 pounds.

: Start with a solid chunk of 7075 aircraft aluminum, here scribed for cutting slightly oversize

: Blanks are cut to size with thinnest abrasive cutting blade in high-speed angle grinder. I tried using a 12″ cutoff saw, but it couldn’t cut this high-strength aluminum.

: Finished raw blank

: Facing both sides of the blank with carbide-insert face cutter end mill

: Milling holes for bolts to attach to chassis. PDF drawing printed on sticky paper at 1:1 eases the layout and provides a useful double-check against errors.

: Milling the first outside radius on the rotary table.

: Milling the second outside radius

: 45-degree faces are rough cut with the angle grinder, then clevises are supported on V-blocks clamped to the milling machine.

: 45-degree faces milled smooth with face cutter

: Repeat eight times. Ready for slot milling.

: Milling the slots for the rod ends using a ball-end mill.

: Milling holes for the rod-end retaining bolts

: Milling an additional relief for the rod ends. Test assembly showed interference, so I went back to the computer model and, sure enough, there it was. Now I know to use the interference and clearance detection tools.

: Finished lower A-arm clevises. Outside radius on front was also cut on the rotary table / milling machine.

: Lower suspension attachment clevis assembly drawing

After playing around with various kinds of hole cutters, mills, angle vises, and so on, I’ve settled on the best method for cutting fishmouths in tube ends so they fit together properly when building a tube frame with round tubing. Since the tubes will be welded they don’t have to be perfect as you would get by using a milling machine. Also, the typical joint has several tubes meeting which need to accomodate each other, and on a milling machine this would take a separate setup for each tube at each joint, taking an inordinate amount of time. Forcing Solidworks to show the correct shape of the ends of each tube requires some real work, an explanation of which I found over on the LoCost website. I’m going to provide a modified and updated tutorial here.

The first thing to understand is that each tube must be fully welded before adding the next tube. This makes the finished structure much stronger than if you tacked all the tubes in place and simply welded around the remaining visible joints. Here’s an example:

In a multi-tube intersection, the first two tubes are fully welded before adding the next tube

Third tube in place before welding

Third tube fully welded

Solidworks Tutorial

Although the following tutorial may look long and complicated, once you understand what’s going on each step will only take seconds. And believe me, it’s much faster than grinding a tube to fit using trial and error. More accurate, too.

First, create a weldment profile with the correct outside diameter, a thickness of 0.1mm, and a gap of 0.1mm as shown.

Original weldment use a profile of 25.4 x 1.0 mm round tube

Replace this with the new, slitted profile

Each tube will need to be trimmed to the tubes around it, reflecting the order in which they will be assembled. Insert > Weldment > Trim/Extend. Check your trims.

Select the tube, right click and choose "Insert into new part".

Save the part with a descriptive name. I keep a separate directory of tubes.

Select an INSIDE EDGE and click Insert>Sheet Metal>Bends.

Just click the green check mark. No need to fiddle with any options.

Right click on "Process Bends" and choose "Suppress".

And you get a flat sheet.

Select he surface and choose a normal view

With a Normal View, dimensions and shapes will be correct.

Open a new drawing and insert the current model view.

Set drawing scale to 1:1, full scale

Right click on the drawing view and choose Drawing Views > Rotate View.

Through trial and error, figure out how much to rotate the view so that it is horizontal.

Now we have a horizontal drawing view.

Insert another drawing view...

Also of the current model view.

Rotate the view as before to get another horizontal view.

Two views on one drawing.

Align the views horizontally by right clicking on one view and choosing Drawing Views > Align Horizontally by Origin.

Crop each view by first drawing a rectangle with 4 lines. The automatic draw rectangle won't work because it uses the unrotated axes.

Crop the view by selecting the four lines of the rectangle, right click and choose Drawing Views > Crop View

Now we have both tube ends with the middle removed, fitting on a single A4 sheet.

Now we need a reference for how far the ends of the tube are from each other. Go back to the tube part and create a sketch like this.

Using the sketch, extrude a cut through the part and keep all bodies.

The part now looks like this.

Go back to the drawing and add annotations as necessary for use in the shop.

Save the file as a PDF and print it out on sticker paper. Cut out the 2 ends and stick them on the tube at the indicated distance. Use an angle grinder to grind to the lines.

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