Most problems in tube bending are not problems of the machine. They are problems of the drawing. A radius that no die can form, a straight too short for the clamp, two radii where one would do, a tolerance that asks for more than the process can hold, a rotation that makes the part hit the machine. Each of these can be found on paper in minutes, and each costs far more to find on the shop floor, after tooling has been cut and tube has been scrapped.
This article collects the tube bending design guidelines that make a tube part bendable. It is written for the designer or engineer who draws the part, and for the buyer who reviews the drawing before a quotation. It explains the reason behind each rule so that it can be applied with judgment, and it gives starting points that the supplier should confirm. The process behind the rules is in rotary draw bending, and the tooling is in tube bending tooling and how to match a die set to the job.
Tube Bending Design Guidelines, Rule One, Standardize the Centerline Radius
A bend die is cut for one radius, so every different radius on a part is another die set. The cheapest design change is to use the same radius for every bend on a tube, and the same few radii across a family of parts. A single tube should use one radius on all its bends whatever the angle, provided no bend exceeds 180 degrees. Across a family, two to four radii per diameter is usually enough, such as 2D, 2.5D, 3D and 4D, and the ladder should stay short. The full treatment is in tube bend radius standards and how to choose a radius.
Keep the radius at about 2 to 2.5 times the outside diameter or more, unless there is a clear reason to go tighter. Below that the cost of tooling and scrap rises quickly, and thin wall may not be formable at all. State the radius as a centerline radius, which UK and Australian drawings call the centreline radius, and give the ratio in brackets so that the intent is clear. The definition is in centerline radius explained for tube bending.
Rule Two, Leave the Minimum Straight Length
The machine has to grip the tube somewhere, and the part has to give it room. Between two bends there must be a straight long enough for the clamp die and for the tooling to clear the previous bend as the tube rotates. A common working minimum for the clamp die is two times the outside diameter, and three times or more on thin wall, tight radii or any job with a mandrel. That sets a starting point for the minimum straight length between bends, and the supplier should confirm it for the machine and the tooling.
The ends need the same thought. The first bend needs a tail long enough to be clamped, and the last bend needs enough tube beyond it to be held and, where there is a mandrel, supported. If an end must carry a feature such as a flare or an expansion, that adds length, as covered in rule six. The rule of thumb is to ask the supplier for the minimum straight at both ends and between bends before the drawing is released, and to design with a margin.
| Location | Starting point | Why |
|---|---|---|
| Between two bends | At least the clamp die length, commonly 2 to 3 times the diameter | The clamp needs somewhere to grip and the tooling must clear the last bend |
| Before the first bend | Enough tail to clamp, plus the feed reference | The machine clamps and feeds from this end |
| After the last bend | Enough to hold, and to support with a mandrel | The tube must remain clamped through the bend |
| Beside an end form | Extra length for the forming stroke | The end former needs clear tube to work on |
Short straights are the most common reason a part cannot be made as drawn. When a drawing puts two bends closer together than the clamp length, the answer is a modified clamp, a different sequence, or a redesign, and redesign is far cheaper at the quotation stage than after tooling is cut.
Rule Three, Keep Every Bend Inside the Machine Angle
Every bender has a maximum bend angle, and the bend has to be made with a margin for springback. Telhoo publishes 190° on its CNC range and on models such as the 219NC and 185° on several NC models, so a 180° return bend can be over-bent by a few degrees. A design that asks for an angle at the very limit leaves no room to compensate. Check the largest angle on the part plus the expected springback against the maximum angle of the machine.
Also state the angle as the bend angle, which is the change of direction, and not the included angle between the legs. A part whose legs form a 120° included angle is a 60° bend, and reading it the wrong way round is the most common calculation error in the trade. The arithmetic is set out in pipe bending calculations, and the springback side in springback compensation tube bending and how to prove it.
Rule Four, Reduce Plane Changes and Check Clearance
Every change of plane between bends is a rotation of the tube, and every rotation is a chance for a position error that grows along the part. Design with as few plane changes as the function allows, and keep the angles between planes to simple values where possible. A planar part, with all bends in one plane, is the easiest to make and to check.
Three-dimensional parts also have to clear the machine. As the tube is bent, the finished portion swings through space, and it can collide with the bender, the mandrel carriage or the pipe support. A design that looks fine on screen may not be formable in the order it needs. Ask the supplier to check the sequence, ideally with 3D bending simulation that reads the CAD file, which Telhoo lists on its CNC models. Where a collision exists, a change of bend order, a longer tail or a redesign usually removes it.
Rule Five, Put Tolerances Where They Matter
A tube part is assembled by its ends and its fixing points, and not by its individual bends. The tolerance that matters is therefore the position of the ends and the key features relative to a datum, and tolerancing every angle tightly adds cost without adding function. Errors stack along a multi-bend part, so an individual bend held to a tight angle can still put the last end outside the fixture. Specify the end points against the fixture datums, and let the bend angles follow from that.
State the quality limits the process can address. Give the maximum ovality and where it applies, since a bend near a fitting or a seal is held tighter than one in a straight run. Give the minimum wall after bending, or the maximum thinning, and say where it is measured. If there is a pressure or fatigue code, name it. These limits decide the radius, the wall and the tooling, and a drawing that leaves them out leaves the supplier to guess. The wall side is in tube bending wall thickness and the wall factor.
Designing for Inspection and for Cost
A part that is easy to bend should also be easy to check. Give the checking method on the drawing where it matters, such as a fixture, a template or a measuring arm, and place datums where a fixture can locate them. A part that can only be measured on a coordinate measuring machine is slow and expensive to check in volume. A part with a simple fixture can be checked at the machine in seconds, and that keeps the process under control through a run.
The same attitude applies to cost. The cost of a bent part is made up of tube, tooling, machine time, scrap and inspection, and the design sets most of them. A short radius ladder reduces tooling. Generous straights reduce scrap. Fewer plane changes reduce cycle time. Tolerances on the end points reduce inspection effort. A design review against these tube bending design guidelines before the quotation request is the cheapest cost reduction available, because it costs only time.
Common Drawing Mistakes the Guidelines Prevent
The same mistakes appear on drawing after drawing. The first is a radius that is really an inside radius, which gives tooling tighter than intended. The second is a nominal pipe size used as if it were the outside diameter. The third is a bend angle given as the included angle between the legs. The fourth is a straight length shorter than the clamp. The fifth is a tolerance on every bend and none on the end points. The sixth is a mixture of apex and tangent dimensions in one drawing. The seventh is a three-dimensional part drawn with no check that the tube can be bent in the order it needs.
Each of these is a statement that the drawing makes without meaning to. A radius with no reference surface says nothing about which radius is meant. A tube size with no tolerance says nothing about the bore the mandrel has to fit. Reading the drawing as a supplier would, asking what each number commits the process to, finds most of them. It is also a good habit to have someone who has not seen the part read the drawing cold and list the questions they would ask.
Allowances for Cut Length and Trim
The cut length of the blank follows from the bend schedule, as the sum of the straights plus the bend allowances, and the first article confirms it. Designers can help by allowing for a trim where the ends are critical. A tail left a little long, and trimmed after bending, gives a clean and accurate end and avoids having to hold a short tail during the bend. That costs a cutting step, and for parts with tight end tolerances it is often cheaper than scrap.
Also allow for the effect of springback on the position of later features. If the first bend relaxes by a degree or two, every later feature rotates with it, and the correction is made per bend. The part must be designed so that the end features can still be located within tolerance after those corrections. The method is in the calculations article linked above and in the springback article.
Designing Parts for Loading and Automation
If the part will run on an automated line, the design should help the handling. Parts with a consistent length and a stable center of gravity are easier for a robot to pick and place. Welded tube may need a seam position to be controlled, since a loader with seam detection can orient it, as in automated tube bending cell and where the time goes. Heavy parts need handling points. A drawing that considers how the part will be gripped and moved saves trouble when the volume rises and the line is automated.
Rule Six, Keep Tube Ends Clear of Bends
Many parts carry an end feature after bending, such as a flare, an expansion, a reduction or a bead, and the end former needs clear tube to work on. A bend placed too close to an end form narrows the process window, because the wall thinning already spent in the bend helps decide whether the end forms cleanly or splits. Leave enough length between the last bend and the end feature, and ask the end forming supplier for the minimum.
Ends also need preparation. Cut ends should be square and free of burrs, and where welding follows, beveled or chamfered as the weld requires. Telhoo’s tube end forming machine and pipe chamfering machine ranges cover the operations, and the cutting station that supplies the blanks is the automatic pipe cutting machine range. Blank length accuracy sets the first straight of every part, so a consistent cut is part of the design.
Rule Seven, State the Dimensioning Convention
Bent tube is dimensioned three ways. Apex to apex extends the centerlines until they intersect, tangent to tangent gives the true straight sections, and XYZ coordinates give the positions of the intersection points. The formulas differ with the convention, and mixing them double-counts the arc or ignores it. State which convention the drawing uses, and give the bend schedule in a form the machine can use, as the feed, rotation and angle for each bend, or as XYZ points. Telhoo’s CNC pages list input as either form.
Give the radius to the centerline and not to the inside or outside surface, and give the tube outside diameter as the real diameter and not the nominal pipe size. A 2 inch nominal pipe is 60.3 mm outside, not 50.8 mm, and the difference is enough to ruin a radius. These small statements on a drawing prevent most of the questions that otherwise delay a quotation.
Rule Eight, Choose the Wall, Material and Symmetry With Bending in Mind
The wall and the material decide how hard the bend is, and the choice belongs at the design stage. A wall factor, which is the diameter divided by the wall, above about 30 needs a mandrel, and above about 40 needs a multi-ball mandrel and wiper. A hard temper may crack on a tight radius. Stainless needs more force and aluminum springs back further. The comparisons are in aluminum tube bending and how tube metals compare, and the support needed in types of mandrels for tube bending and how to select one.
Symmetry is a design choice that pays. Mirrored left and right parts can run on one machine with bending in both directions, and symmetrical U-shaped parts can use a double head bender that forms both ends in one cycle. A design that keeps the two halves identical saves tooling and time. The comparison of methods and machines is in tube bending methods compared and when each fits.
A Redesign Example
This example is illustrative and is not a customer drawing. A frame member in 38.1 mm tube has four bends. The original drawing uses three different radii of 70, 90 and 110 mm. The straight between the second and third bends is 40 mm, and the last bend is 15 mm from the end. The tolerances are ±0.5° on every bend. A review against the rules finds four problems.
| Item | Original | Problem | Revised |
|---|---|---|---|
| Radii | 70, 90 and 110 mm | Three die sets, and 70 mm is 1.8D | One radius of 95 mm, which is 2.5D |
| Straight between bends 2 and 3 | 40 mm | Shorter than the clamp, which is 76 to 114 mm | 80 mm |
| Tail after the last bend | 15 mm | Too short to hold | 60 mm, trimmed after bending if needed |
| Tolerance | ±0.5° on each bend | Asks more than the stack needs | End points to datum, angles follow |
The revised part needs one die set instead of three, can be clamped at every bend, and is tolerance-checked in a fixture. None of the changes alters the function of the frame, and together they turn a part that could not be made as drawn into a routine job. The clamp length figures come from the common working minimums of two to three times the outside diameter, which is 76.2 to 114.3 mm for 38.1 mm tube, and the supplier should confirm the real values for the machine and tooling.
How to Use the Guidelines With a Supplier
The guidelines work best as the start of a conversation and not as a set of absolute limits. Every number in them is a starting point, because the real minimum straight, the real tightest radius and the real angle limit depend on the machine, the tooling, the material and the wall. The sensible routine is to send a draft drawing early, ask for a feasibility review, and agree changes before the drawing is released and before tooling is ordered. A supplier who builds the machines can say quickly which rules bind your part.
Ask three questions at that review. Can every bend be made in the order drawn, with the straights available? Which tooling will it need, and how many die sets? And what first-article and inspection method will confirm the part? The answers become part of the specification. Where a rule cannot be met, ask what would make the part easier, and what it would cost to keep it as drawn. Often a few millimeters of straight length or a change of radius settles the matter.
Keep the review on record. A drawing that has been reviewed against the tube bending design guidelines, with the supplier’s comments and the changes made, is far less likely to cause arguments later, and it forms the basis for the first article and the stored program. For the machines themselves, the ranges are on the NC semi-automatic tube bender and CNC automatic pipe bending machine pages.
A Checklist Before Release
- One radius per tube, from a short ladder, at about 2 to 2.5 times the diameter or more.
- Straights of at least the clamp length between bends and enough tail at both ends.
- Every angle inside the machine maximum with room for springback.
- Few plane changes, and the sequence checked for collisions.
- Tolerances on the end points to a datum, with ovality and wall limits stated.
- Clear tube beside every end feature.
- The dimensioning convention, the centerline radius and the real outside diameter stated.
- Wall and material chosen with the wall factor and the radius in mind.
Send the drawing with those answered, following the tube bending design guidelines above, and a supplier can quote without a second round of questions. A drawing prepared this way also shortens the time from enquiry to first article, because the feasibility questions have already been asked and answered. Send us the part drawing, and we will say where it works as drawn and where a small change would help. The machine side of the same decision is in how to choose a tube bender from the part drawing, and the wider options are on our tube bending solutions page.
