Buyers who ask for precision tube bending usually want one number, a tolerance the machine can hold. There is no single number, because a bent tube is a chain of features and each has its own tolerance and its own way of going wrong. The angle of one bend is easy to hold. The position of the far end of a six-bend part is hard, because it depends on every angle, every length and every rotation along the way.
This article separates the tolerances, shows how errors stack with a worked example, explains the difference between machine repeatability and part tolerance, and gives a method for specifying and checking them. It uses Telhoo’s published repeatability figures as the reference. The geometry of the radius is in centerline radius explained for tube bending, and the corrections that keep angles on target are in springback compensation tube bending and how to prove it.
The Six Tube Bending Tolerances
Each tolerance describes a different kind of error, and each has a different cause. Treating them as one leads to drawings that ask for the wrong thing.
| Tolerance | What it describes | Main cause of error | Usual gauge |
|---|---|---|---|
| Bend angle | Direction change at each bend | Springback, clamp slip, control | Protractor, template, fixture |
| Centerline radius | Radius of each arc | Die radius, springback opening the arc | Template, measuring arm |
| Ovality | Roundness of the section at the bend | Missing support, worn tooling | Micrometer, ring gauge, plug gauge |
| Wall after bending | Thickness left on the outside | Radius ratio, pressure die, mandrel | Ultrasonic gauge, sectioned sample |
| Straight lengths | Distance between and beyond bends | Feed accuracy, cut length | Caliper, fixture |
| End position | Where the ends and fixing points sit | Stack of all the above and of rotation | Checking fixture, measuring arm |
The first four are properties of a single bend. The last two are properties of the whole part, and they are the ones an assembly depends on. A part can pass every bend check and still fail the fixture, which is why the end position is the tolerance that decides.
Machine Repeatability Is Not the Same Thing
A machine specification lists repeatability, which is how closely each axis repeats a commanded value. Telhoo publishes ±0.1° for bending and rotation and ±0.1 mm for feed on its CNC range, and ±0.1° bend angle on its NC range. Those figures describe what the axes do. They do not describe what the part will measure, because the part also depends on springback, material variation, tooling wear, lubrication and the measurement method.
A useful rule is that the part tolerance a process can hold is always looser than the repeatability of its axes. How much looser depends on how many bends the part has, how long the legs are and how well the springback correction is proven. Tube bending tolerances on a part should therefore be agreed from a trial on real tube, and not read from the data sheet. Repeatability is the foundation, and the trial shows what is built on it.
How Tube Bending Tolerances Stack Along a Part
The position of an end depends on every bend before it, and an angle error at an early bend is multiplied by the length of tube that follows. A small angle error at the first bend moves the far end by roughly the remaining length times the error in radians. Errors at later bends act on shorter lengths and matter less.
Here is a worked example using assumed values. A part has four bends with the remaining lengths to the far end of 1,200, 900, 600 and 300 mm. Suppose each bend has an angle error of 0.5°, which is 0.00873 radians. The contribution of each bend to the end position is the remaining length times that error.
| Bend | Remaining length | Error at ±0.5° | Error at ±0.1° |
|---|---|---|---|
| 1 | 1,200 mm | 10.5 mm | 2.1 mm |
| 2 | 900 mm | 7.9 mm | 1.6 mm |
| 3 | 600 mm | 5.2 mm | 1.0 mm |
| 4 | 300 mm | 2.6 mm | 0.5 mm |
| Worst case, errors all the same way | None | 26.2 mm | 5.2 mm |
| Statistical, root of the sum of squares | None | 14.4 mm | 2.9 mm |
The lesson is the scale. At ±0.5° on each bend the far end can be 14 mm off in a typical case and 26 mm off in the worst case, which is outside most fixtures. At ±0.1° the same part is 3 mm off in a typical case and 5 mm in the worst case. The figures are illustrative, and rotation errors add to them on a part with plane changes. The point is that a part with several bends needs axis repeatability much finer than the end tolerance it must meet, and that is the case for programmed axes on multi-bend work.
Angle and Radius Tolerances
The bend angle is the tolerance most often quoted, and the one that springback attacks first. A tight angle tolerance needs a proven over-bend, stored per bend and per material lot, and axes that repeat the angle. Telhoo’s CNC range lists a bending precision of ±0.1° and a maximum angle of 190°, so there is room to over-bend. The NC range lists ±0.1° and 185° on several models. A machine that stops at exactly the target angle cannot compensate.
The radius is held mainly by the die, since a bend die is cut for one radius, and then opened a little by springback. UK and Australian drawings call it the centreline radius. A tolerance on the finished radius is rarely needed, except where the bend must clear a nearby surface, and where it is, the trial piece should be measured for the actual radius and not only the angle. Asking for a tolerance tighter than the die and springback can deliver adds inspection effort and no function.
Ovality Among the Six
Ovality is the flattening of the round section at the bend, measured as the maximum diameter minus the minimum diameter over the nominal, multiplied by 100. It is the tolerance that fails parts at incoming inspection, because it is easy to measure and it stops joints sealing. The limit depends on the part. A bend near a slip joint, a seal or a flange is held tighter than one in the middle of a straight run.
Ovality is controlled by tooling and not by machine size. The mandrel supports the bore, the pressure die holds the tube in the groove, the wiper fills the gap at the inside tangent, and the fit of the die cavity to the real tube matters. A thin wall raises ovality, and a heavy wall lowers it. If a drawing asks for both a thin wall and a tight ovality limit, it is worth asking whether either can be relaxed. The factors are in tube bending wall thickness and the wall factor and the support in types of mandrels for tube bending and how to select one.
Wall Thickness After Bending
The wall on the outside of the bend thins, and a first estimate is 100 ÷ (2 × CLR/OD + 1) percent, which is 20% at 2D and 14% at 3D. A tolerance on the wall after bending is a minimum remaining wall, or a maximum percentage of thinning, and it has to be measured with an ultrasonic gauge or on a sectioned sample at the tangent points and at about 45° and 90° through the arc. It is a limit that the radius, the starting wall and the tooling jointly decide, and a drawing that sets it must be consistent with the tube ordered.
Where a pressure code applies, the code sets the limit, and it belongs on the drawing. The process then works backward from that limit to the radius and the starting wall. For furniture and decorative work the wall limit is usually a strength question, and a design wall that already allows for the thinning avoids the surprise.
Straight Lengths and End Positions
Straight lengths are held by the feed axis and by the accuracy of the cut blank. A CNC feed with ±0.1 mm repeatability can hold lengths well, and an NC machine where the operator sets the feed holds them as well as the operator and the stops allow. The blank itself matters, because the first straight carries the error of the cut. An automatic cutting station that holds a consistent length and a square end removes a class of error before the bend begins.
The end position is the tolerance the assembly sees. It is best specified relative to a datum scheme that matches how the part is held in the fixture, with the ends and fixing points as the controlled features. That is far more meaningful than a tolerance on each bend, and it lets the supplier choose how to meet it. The checking fixture is where the tolerance is proven, and it should be agreed before production begins.
Rotation and Plane Tolerances
On a part with plane changes, the rotation of the tube between bends is a tolerance of its own, and an error in it acts like an angle error that swings the rest of the part out of plane. A rotation error of half a degree at the first bend moves the far end sideways by the remaining length times the error, just as an angle error does, and the two add in a way that depends on the geometry. That is why a three-dimensional part is harder to hold than a planar one with the same number of bends.
On a CNC machine the rotation is a programmed axis, and Telhoo’s pages list a rotating precision of ±0.1° across the range, with rotating speeds of 25 to 180°/s on the 75CNC. On an NC machine rotation is set by hand, and the operator’s care decides the result, unless the optional electric rotation is fitted. The comparison is in CNC vs NC pipe bender and how to choose. For parts with several planes, the rotation tolerance and its checking fixture should be agreed before the first batch.
Tolerance Expectations by Application
Different industries ask for different things, and the table gives the direction and not the numbers. The right tolerance for a part always comes from its function and from a trial on real tube.
| Application | What usually governs | Typical emphasis |
|---|---|---|
| Automotive tube assemblies | Fixture and clash envelope | End positions to datum, repeatability across a run |
| Furniture and fitness frames | Appearance and fit at joints | Symmetry and surface, then end position |
| Boiler and heat exchanger coils | Header pitch across many returns | Cumulative angle error and pitch |
| Marine and heavy pipework | Fit-up to an as-built structure | Ovality at flange faces, wall after bending |
| Handrail and structural frames | Site fit and geometry | Overall shape, with loose tolerances on single bends |
Each row has a different cost of being wrong, and a different gauge. The applications are compared in tube bending applications by industry and what each needs, and the automotive side in automotive tube bending by part family and volume.
Measurement Uncertainty and Gauge Checks
A tolerance can only be controlled if it can be measured with an uncertainty well inside it. If a part has to be within ±1 mm at the end, the checking method needs to be good to a small fraction of a millimeter, and the fixture or arm must be calibrated and used consistently. A measuring method that scatters as much as the tolerance cannot tell a good part from a bad one, and it makes the process look worse than it is, or better.
Check the gauges on a schedule. Fixtures wear at their locating points, protractors drift, and a template can be damaged. Check the way the part is placed too, since a part that is not seated the same way each time reads differently. Where a result matters, have two people measure the same parts and compare, which shows how much of the scatter is the process and how much is the measurement. The effort is small, and it prevents arguments with a customer about whose measurement is right.
Reducing the Stack Without Tightening the Machine
Several design and process choices reduce the stack of errors without asking more of the axes. Shorter legs reduce the lever arm, since the end moves by the remaining length times the angle error. Fewer bends reduce the number of contributions. Bending the longest legs last, where the sequence allows, reduces the length on which early errors act, though many parts fix the order. Placing the controlled features near the clamped end rather than at the far end shortens the chain between the datum and the feature.
Process choices help as well. A first-article correction per bend removes the systematic part of the error and leaves the random part. A stable lot of tube, consistent lubrication and tooling in good condition reduce the random part. A fixture check on a sample through the run catches drift early, and a feedback to the program corrects it. Trimming a tail after bending gives a clean and accurate end when the end feature is critical.
These measures for tube bending tolerances are cheaper than buying a more accurate machine, and they work with any machine. The design side is in tube bending design guidelines for bendable parts, and the proving procedure in the springback article.
How Tight Is Realistic
It depends on the part, and no table of tube bending tolerances can say. The factors that decide are the number of bends, the length of the legs, the plane changes, the material and its lot variation, the wall, the radius ratio, and the control. A part with two bends in one plane on thick-wall tube can be held tightly. A part with eight bends in three planes on thin stainless is much harder. Programmed axes, a rigid frame, proven tooling and a stored correction all improve what can be held, and none of them removes the need for a trial.
A good habit is to ask for a capability study on a trial run. Bend a number of parts in sequence, measure the key features, and look at how the results scatter and whether they drift. A process that holds the end position well inside the fixture with room to spare is capable. One that only just meets it on the first article will not on the thousandth. The records from the study become the evidence that the tolerance is real.
What a Capability Trial Looks Like
A capability trial is a short, structured run. Bend a sequence of parts, for example thirty in a row, on the production machine with the production tooling, lubricant and speed. Measure the key features of each part with the agreed method, and plot the results in order. The picture shows two things. The scatter shows how repeatable the process is. The trend shows whether it drifts with oil temperature, tooling wear or a change of tube lot.
Compare the scatter with the tolerance. If the whole spread sits well inside the limit, with room on both sides, the process is capable of holding it. If the spread fills the tolerance, parts will be near the limit all the time and some will fall outside. If the average sits off-center, a correction can move it, and if the scatter is wide, the cause has to be found in the tooling, the lubrication, the tube or the clamp. The result is a record that can be shown to a customer and repeated on later lots.
Agreeing Tolerances Between Buyer and Supplier
Tolerances work best when they are agreed and not imposed. The buyer knows what the assembly needs, and the supplier knows what the process holds. A short discussion before the drawing is released, with a trial on a sample part, usually finds a tolerance both sides can live with, and it often finds that a few of the tolerances on the draft can be relaxed or moved. The agreement should name the features, the limits, the datum scheme, the gauge and the sampling plan, and it should be kept with the part number.
Review it after the first batches. If the data shows more room than expected, the tolerance can sometimes be tightened to the buyer’s benefit. If it shows less, the cause can be traced and fixed, or the tolerance revised with a reason. Either way, the agreed record turns an argument about whose measurement is right into a comparison of numbers.
Specifying Tolerances on a Drawing
A drawing should carry only the tolerances that the part needs, in a form the process can use. State the end positions to a datum, the ovality limit and where it applies, the minimum wall after bending, the angle tolerance where function demands it, and the length tolerance on the blank. Give the dimensioning convention, whether apex to apex, tangent to tangent or XYZ, and the centerline radius with the real outside diameter, as set out in tube bending design guidelines for bendable parts.
Leave out tolerances that add cost and no function. A tight angle on every bend of a part that is judged by its end positions is such a tolerance. Where a tight tolerance is needed, say how it will be checked, since a tolerance that cannot be measured cannot be controlled. A drawing that asks for what the assembly needs, and names the gauge, gets a part that fits.
Measuring and Recording the Results
The measurement method matters as much as the tolerance. Use a method with an uncertainty well below the tolerance, and use it the same way every time. A fixture with locating pins and gauges on the ends measures what the assembly cares about and is fast enough to use through a run. A measuring arm or a coordinate measuring machine gives numbers for the record and for the first article. A protractor and a micrometer are good for single features.
Record the results with the part number, the lot, the tooling and the date. A CNC program stores the settings, and the inspection record stores the outcome. Over time the two show how the process behaves, support a tighter tolerance if the data allows it, and answer a customer who audits process control. Telhoo’s pages describe installation, operator training and spare parts support, and say sample parts are bent and inspected before shipment, with a factory acceptance test on request.
What to Send for a Tolerance Review
- The part drawing with the dimensioning convention, the centerline radius and the real outside diameter.
- The tolerances you need, and which are functional and which are habit.
- Tube size, wall and material, with the tolerance you can hold in purchasing.
- Bends per part, plane changes and leg lengths, which set how errors stack.
- The checking method, whether a fixture, template or measuring arm.
- Volume and variants, which decide how much a capability study is worth.
Send those and the reply can say what is realistic and which machine and tooling hold it. Tell us about the part, and see the two ranges on the CNC automatic pipe bending machine and NC semi-automatic tube bender pages. For the wider process view see our tube bending solutions page.
