How to Fishmouth Tubes in Solidworks

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:

Welded Joint

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

Third Tube

Third tube in place before welding

Third Tube Welded

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.

Weldment Profile

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

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

Replace Profile

Replace this with the new, slitted profile

Check Trim

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.

New Part

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

Save Part

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

Sheet Metal Bends

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

Click OK

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

Suppress Bends

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

Flattened Tube

And you get a flat sheet.

Get Normal View

Select he surface and choose a normal view

Normal View

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

New Drawing

Open a new drawing and insert the current model view.

1:1 Scale

Set drawing scale to 1:1, full scale

Rotate View

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

Rotate View

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

Now Horizontal

Now we have a horizontal drawing view.

Insert Another

Insert another drawing view...

Current View

Also of the current model view.

Rotate Again

Rotate the view as before to get another horizontal view.

Two views

Two views on one drawing.

Align Horizontally

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

Draw Rectangle

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 View

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

Shortened Tube

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

New Sketch

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.

Extrude Cut

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

Cut Part

The part now looks like this.

Drawing Annotations

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

Save as PDF

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.

2 responses to “How to Fishmouth Tubes in Solidworks

  1. Good day Sir,

    Well done on the tutorial. I have had to figure out that tubing notch method on SolidWorks as well. It’s nice to know that others use this method!

    Thank you for posting about this project as it has helped me to know of things that I am on track with and things to consider.


  2. There is an easier way… software by BendTech. Not only can you easily design your tubular chassis (and sheet metal) and rotate it in 3D, but included are tools to specify the order of tubes in each joint and to print templates which wrap around each tube to cut… very cool. They also have tools included to tell you exactly how to make any bends for bent parts. I could go on and on, but it has everything you need for design and it’s very easy to use. I’ve been a user for 10+ years… and the underlying CAD system is Solidworks.

    Check it out at inexpensive (but very valuable) software for anyone that wants to build a tube chassis. They have done an amazing job.

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