Tolerance Profile Surface or Profile Line 5

[Luisen]

Hello everybody, who know wich is the diference between Profile Surface or Profile Line, i know Profile Surface, but, iam not sure of Profile line, and i dont know exactly when we must use this tolerance, and how we must apply it.

 

[dingy2]

Profile of a line is not used that much but I have seen a couple of examples over the years.

In a stamping operation, profile of a line (2 dimensional) is used show the shape of the blank in critical areas. It is understood that the dimensions are taken at the cut and not the break. It is measured at the edge of the part.

I have also seen profile of a line utilized on a section of a door seal. By section, I mean that a slice 90 degrees to its length is taken and mounted. Using a Optical Comparitor (shadowgraph) one can compare the outline of the shape to a template with the inner and outer boundaries of profile of a line reflected. It the section was within the boundaries, the part conforms to requirements.

Hope this helps

DD

 

[Heckler]

"The concept for profile of a surface and profile of a line are identical, with the exception that profile of a surface is a three dimensional and profile of a line is two dimensional. Profile of a line is often used in conjunction with profile of a surface. For example, profile of a surface deines the shape or location of the feature, and profile of a line is used to refine the feature in one direction, as in extruded parts." Al Neunmann

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[ctopher]

I agree with Heckler. I have worked with inspectors that don't understand the difference and will use either.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[AliThePro]

The difference between profile of the surface and profile of the line is similsr to the difference between flatness and straightness applied to a surface. If flatness tolerance is .2 then the whole surface must be between two planes that are .2 apart. If, on the other hand straightness with .2 tolerance is applied to the surface, then every line in the direction shown must be straight within .2 tolerance and the whole surface does need to be within .2 tolerance. That is a surface which is sort of wavy in the direction normal to the view, but with line elements straight within .2 in the direction shown in the view is acceptable. Line profile applies to a line where surface profile applies to a surface. Hope this is helpful.

 

[MechNorth]

Exactly, Ali. Well done.

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

 

[hjmmjm]

I have a question regarding the proper way to report profile of a line. I need to layout a part for a German company. It's my understanding that they asking for actually numbers. I've only inspected profiles using an overlay and comparator and only as attribute data. Pass/fail. I do not have a part sample to use as a nominal. Could someone please enlighten me as to the best way to get them some actual numbers. Thanks in advance

 

[drawoh]

hjmmjm,

I assume your line is a curve of some kind.

You can insert points on your line and attach dimensions to them. This should be easy on any CAD package. This technique is illustrated in several places in ASME Y14.5M-1994.

This all assumes that you do not have an equation or something else that describes your line.

If your line is straight, you can attach X/Y dimensions to each end. If your line is straight and orthogonal, you just use conventional dimensions.

The ASME Y14.5M profile tolerances are functional no matter what your approach. In the case of curves, the old +/- tolerances are practically meaningless.

JHG

 

[hjmmjm]

Thanks. I have it cadded out. Its a curve with 14 XY basics. It's profile of a line w/in 0.1 and it fits within the profile zone on my overlay. I still dont really understand how I can give these guys numbers though. They want to know what the "profile" actually measures. Any ideas? Thanks again in advance.

 

[dingy2]

First of all, if you are using a template, the result is "OK" or "NO OK" since this is an attribute check but templates are most effective as an Operator check at the work station. On sample submission, the Customer usually wants an "actual".

In the automotive supplier base, each dimension on the drawing is numbered. Let's say this profile is number 28. If we have 14 points shown with basic dimensions, letter each one so that we have 28a, 28b, etc.

If we have a profile (surface or line) with 0.1 mm, it defaults to a +/- from the theoretical shown with basic dimensions. The would be +/- 0.05 mm. Using a coordinate measuring machine (CMM), we could show how far the surface is away from each theoretical point.

As an example, 28a could be -0.033 while 28b could be +0.035. This would make the Customer happy.

The absolute best way of measuring profiles on curves, etc. is with a CMM, servo motor and a scan mode. One would feed in the basic dimensions and tolerance. The equipment would create a tolerance zone and scan the surface at predetermined intervals.

Hope this helps.

 

[drawoh]

hjmmjm,

I take it you have numbers for the nominal form of your curve. The GD&T profile tolerance provides a zone that your face must be contained within. A profile tolerance of 1mm states that the tolerance zone is 1mm wide, centred on your nominal position. This completely describes a range of acceptable forms.

It would be possible to go into your CAD drawing/model, and use some sort of offset to show the tolerance zone to scale. You could apply your 14_dimensions to the upper and lower range. This is a complex, obfuscated way to show something GD&T shows clearly and unambiguously.

Who designed the part? Are you trying to explain your design to them, or are you trying to show you can fabricate and inspect their part?

JHG

 

[thundair]

Look at a NASA wing profile it is given in X Y points.

When we check a profile we list the nominal I.E. X=26.829, Y=44.789 and show the actual I.E. X=26.820, Y=44.785.

If there is an error it is shown in the positive or negative and shown normal to contour I.E. Error -.003

Cheers

I don't know anything but the people that do.

 

[hjmmjm]

Thanks all.

This is a "pawl" used in a gear box. It's a pretty simple part to machine really. Lots of radii locations programmed on a machining center. Its for a company overseas that is mandating a mountain of ppwk.

thundair, your error example doesn't compute to me. Is there a formula for that. How is the error calculated? In your reports do you report the deviation off of each X Y nom/act? If so, is the overall "actual" error reported as the average, worst case, range?

I have a CMM so I can generate the data needed.

I'm getting there thanks to you guys.

 

[TomGDandT]

The CMM should have the vector normal to the surface at the measurement point. The difference between the measured point and the nominal point is the important number.
Does this deviation from nominal fit inside the profile tolerance zone? A profile of 0.3 had give you a +/- 0.15 tolerance zone centered about nominal.
Are you measuring relative to the "Datum Reference Frame"?

Tom Rhodes, GDTP-S
QMC LLC;

http://www.qmc.com

Senior Dimensional Management Engineer.
CeTOL 6 Sigma