Proper Method to Produce Lobster-back Duct Bends

One type of industrial component I have been involved with the design and manufacture of is lobster-back bends. This type of duct bend is made up of segments cut from flat sheets or plates, rolled into cylindrical parts, then assembled. These can be light sheet-metal or manufactured from thick plate.

This quick tutorial is a supplement to the one I produced an outline of a method I have used modeling this type of component using Alibre Design. As this supplement concerns producing parts ready for manufacture and applies to whatever software you have used, that is not important as this short tutorial is to outline turning your modeled bend into the flat profile ready to be made into the completed bend.

In this modern world, the bend parts will be cut out using CNC laser, or CNC Plasma cutting machines. Sometimes we produce the nc programs ourselves or we are required to produce the correct files for the laser / plasma department to program and cut out. Making the program to cut out the parts starts normally from a 2D dxf file at a scale of 1 : 1. This is the first part of the process that has to be correct. If you produce this dxf incorrectly the finished parts will be useless. Producing this at the right scale, 1 : 1 is different with different 3D cad applications, other problems can be caused by you working in different drawing units. If you are not doing the program, talk to the person who is to make sure you produce the dxf as required. Having a large quantity of wrongly cut parts is not a good thing

  1. Step 1:

    The image shows a typical duct bend. It is common practice to make the center line radius the same as the duct inside diameter, in this case, 300mm diameter.

    The example bend is made up of 7 segments. Bends made up from 5 segments are also quite common. The end segments are basically the same as one of the middle segments cut in half. The example bend is made up of 7 segments. Bends made up from 5 segments are also quite common. The end segments are basically the same as one of the middle segments cut in half. This arrangement makes the end faces to be east to weld onto the straight cylindrical duct sections between the bends. If your bends are not made this way, the trades-persons assembling this section you have designed will consider you not to be up the task in hand, just another of those useless drawing office staff who don't have the slightest idea of how to do their job properly

  2. Step 2:

    This is the correct way to nest the parts on the sheet. Parts nested this way achieves two desirable outcomes. The first, the pieces fit together efficiently and the second one, speeds up the manufacture process.

    If I am not programming the machine to cut these parts this image shows the dxf profile I will send them, but with a few modifications to make it more useful.

  3. Step 3:

    Once I have made the dxf file, I will open it and make some modifications. The first thing I will do is remove any line on top of another line. This line on top of a line often happens with turning a flattened 3D part into a dxf. The nc code produced to cut the profile often does not like these lines on top of lines. The next modification I do to these bend profiles is a result of what happens to the splines that make up the sine curves in the flattened parts, turn into many short line segments. The nc code produced from this then requires the machine from the x-y coordinate at line start, to accelerate quickly up to cutting speed, stop at the x-y coordinate, then head off to the next x-y coordinate repeating the process at each point. This can get quite hard on the machine, especially plasma machines as cutting speed can be quite fast. With the g-code that most machines use, arcs and circles are way more machine friendly, as these are defined by functions in the code, the machine follows arcs and circles smoothly. I like to replace these short line segments with 3 point arcs that closely match these line segments which i do manually to the dxf file.

    Another modification I make is place short breaks in the sine curve part of the profile and also make them slightly sort of the outside profile of the nested bend parts. This means that the profile stays in one piece so that all of the parts an be put through the plate rolls in one part. The individual parts then have these small tabs cut to separate the pieces. If you supply the workman with individual parts they will probably tack weld these together, roll them, then split them apart. Making a nest of the parts this way reduces the distance to cut compared with individual parts of the bend each separate. With laser cutting the kerf from the cut is usually so small that it can be ignored. Mostly with plasma and gas cut parts it can be also ignored, though if in cases where it matters the dxt file can be adjusted to compensate. Not having had much to do with water-jet machines I do not know if the thickness of the kerf needs to be considered.

    When we design anything we should be also looking into how it will be made. our model should be made to fit in with the manufacture of the completed part. I have been involved with designing and building plant that uses lobster-back bends. Modeling them the way I do, I know will make it a simple process to get the finish part made.