Locating a center line on a rectangular part 1

[tmech77]

I have a rectangular part which has two holes which are to be located symmetrically about the center line of the part. What is the correct way to dimension the hole locations? Should I show the center line, identify it as CL and have a dimension going from the edge of the part to the center line? In other words, is it necessary to dimensionally locate the center line, before I dimension the holes from the center line?

 

[MikeHalloran]

I think the location of centerlines can be implied if they are shown on a drawing, but dimensioning features from centerlines is not good practice, for one because the centerlines don't exist until/unless someone scribes a mark there, for two because the uncertainty of locating the scribe mark adds to the uncertainty of locating the hole relative to the center scribe mark, usually effectively consuming your tolerance.

Just dimension from two adjacent edges. The part doesn't know it's symmetrical, or not.


Mike Halloran
Pembroke Pines, FL, USA

 

[rb1957]

dimension one hole from the edge, note (2 plc).

dimension both from the edge.

dimension one for the edge and dimension the space between the two holes.

what's more critical ?
a) the holes are the same distance from the edge (symmetrical about the CL)
b) the distance between the holes

i agree with mike ... your dimensioning should be to real (usable) datums. i've seen stuff, installed inside an airplane's fuselage, dimensioned to the ground plane !??

Quando Omni Flunkus Moritati

 

[ctopher]

Depends on how you want to tolerance the holes. If you want them at the center, dim the part, draw a centerline thru the center of the part (leave off CL, not used anymore), draw the holes on the centerline.
The machinist will locate the center of the part on the machine regardless of the tolerance, and drill the holes.
The holes are centered in relation of the part size/tol.

Dim from the edge, you get the tolerance from that edge, if that's what you need.

Chris, CSWA
SolidWorks 13
ctopher's home
SolidWorks Legion

 

[Compositepro]

If the edges of the plate are flame cut or the plate is out of square, then it would probably be a good idea to use a centerline as reference.

 

[JohnRBaker]

It all depends on what your 'design intent' is. Is the relationship of the holes with respect to the centerline more critical than to the edges of the plate? If so, then that's the way it should be dimensioned.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[KENAT]

What drawing standards do you work to?

At least some of the above suggestions are possibly not in compliance with ASME Y14.5.

Per ASME Y14.5M-1994 center lines by themselves imply nothing - there is no assumed tolerance just from showing features aligned or symmetrical...

You're a bit brief on functional requirements but you might consider making the width of the part a datum feature. Then you can locate the holes on its center plane which is effectively the datum plane - indicating this graphically by use of a center line (none of the overlapping CL nonsense by the way). In order to indicate how far from the center line it can vary I suggest considering use of position tolerance to control location of the holes.

This kind of question is probably better off in forum1103

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[FACS]

I just did this yesterday.

If symmetry is the most important feature, and the part overall dimension has a lower tolerance, then this is what we do:

We use the center line of the part, and have a small centering drill make a spot. This spot is programmed as Zero. It now is a feature that can be seen and programmed. It's sometimes most important when we are making prototypes, and if for some reason the part has to change a overall dimension to fit a fixture, then the hole to hole locations are symmetrical, and the part is not ruined.

Everything is then dimensioned from this zero point. We do this because mounting the part from these two holes is critical and the hole-to-hole location is important. When it is set up in the CNC, the machinist has to know why we are doing this otherwise he will program the machine from the top and far corner of the overall part. Then we end up with a tolerance stack that we are trying to avoid.

Of course, we are allowing a small center drill to make a mark on the part that QA can use for datum point. Sometimes a mark is not allowed so....

The best bet is to talk to the machinist or CNC programmer, and explain to them what you are trying to achieve. I know that if my machinist decides to just use the edges, then the part won't work as intended. All machines have a tolerance based on length traveled... the less travel you have, the closer the part will be to your tolerance.

Charlie

http://www.facsco.com

 

[benta]

I'm not a professional technical draftsman, but I believe KENAT is, so listen to him.

But generally, it is best to dimension/tolerance a drawing so that you can actually measure these when holding the workpiece in your hand. Dimensioning to an imaginary line/feature somewhere is looking for trouble. It should be possible to check the part using calipers/micrometer/pins etc.

Cheers,

Benta.

 

[MikeHalloran]

The last place I worked had a Trumpf CNC punch that could, if you programmed it to, draw a centerline on a part, using a super high speed marking punch that could also draw characters or arbitrary graphics. We used that feature to mark part numbers on the resulting blanks.

However, like any CNC sheet metal tool of which I am aware, it grasped the actual sheet and located it against two edges that were part of the punching machine's traveling carriage. It did not care if the sheet edges were flame cut or sheared; it was left to the operator to make sure that the sheet was large enough to provide stock so that the rectangular punches that defined the programmed blank edges were not asked to nibble the edge of the sheet.



Mike Halloran
Pembroke Pines, FL, USA

 

[tbuelna]

A drawing should be thought of as a set of inspection requirements, rather than manufacturing instructions. In these terms, it would make sense to use the two hole cylinders (ie. one hole is datum A and the other is datum B) to establish a datum defining the plane of symmetry (A-B). The outer surfaces of the part would then be located with basic dimensions and profile tolerances relative to datum A-B. That would account for all geometric factors in the outer part surfaces, such as taper, parallelism, etc.

KENAT is basically correct in that it is bad drawing practice to use a CL as a datum. Datums should always be established from surface features that can be measured. However, it is possible to accurately establish the datum plane A-B through the two hole cylinder axes using a CMM, or less precisely with an inspection fixture using a pair of diamond pins that locate off the hole sides in one direction.

 

[KENAT]

tbuelna - I considered suggesting what you say about using the hole pattern as the datum.

However, since the OP doesn't give much information on function and hasn't come back to clarify it's difficult to say for sure which approach is more appropriate.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[tbuelna]

KENAT-

Attached are examples of two different approaches for establishing a datum frame for the situation under discussion. The first example uses a basic dimension applied to opposing sides of the part as the datum. Here the datum plane is implied as the mean between the part sides taking into account their surface irregularities, and the holes are located relative to the part sides. The second example uses two hole cylinder axes and a basic dimension between them to establish an orthogonal datum frame. Here the outer profile of the part is relative to the two holes.

Either approach is acceptable. But as you note, factors such function or manufacturability would determine which is more appropriate.

Regards,
Terry

 

[Tunalover]

I agree with Kenat. The simplest approach is to assign a datum to the width dimension. This creates a datum reference plane right in the middle. Draw a center line there then dimension to your heart's content. That datum will probably be the secondary datum in the feature control frame.

Tunalover