WF4 leading/trailing zeros

[amedina]

So my company wants to have the diameter/radius call out dimension have a
leading 0 before the period on dimensions smaller than 1mm

Similarly we want basic dimensions to have at least two trailing zeros to
make sure no digits were missed.

so for example a diameter would be 0.57 rather than .57 and a basic
dimension of 15.0300 rather than 15.03 and similarly 15.00 rather than 15


Any idears of how this sort of thing can be controlled. If you got some sort
of document too about this, shoot it my way, I'll make good use of it.

regards,

Alfonso

[ikamster]

In the config.pro there is an option for default_dec_places, and then in PROPERTIES>Drawing Options you can set the lead_trail_zeros option.

[davehaigh]

Some of what your company wants you to do meets the standard, some of it doesn't.

Here's what ASME Y14.5-1994-r2004 says:

1.6 TYPES OF DIMENSIONING
Decimal dimensioning shall be used on drawings
except where certain commercial commodities are
identified by standardized nominal designations,
such as pipe and lumber sizes.
1.6.1 Millimeter Dimensioning. The following
shall be observed where specifying millimeter di-
mensions on drawings:
(a) Where the dimension is less than one millime-
ter, a zero precedes the decimal point. See Fig. l-2.
(b) Where the dimension is a whole number, nei-
ther the decimal point nor a zero is shown. See Fig.
l-2.
(c) Where the dimension exceeds a whole number
by a decimal fraction of one millimeter, the last digit
to the right of the decimal point is not followed by
a zero. See Fig. l-2.

[mlocascio]

Good information to have!

[amedina]

Yeah, The info is good. We had already looked into this before. Terry
Johnson had posted the information on how to control the leading and
trailing zeros before in WF2 I believe. However, I thought maybe it would be
a good thing to bring up again to see if any progress/change had been made.

I think there is confusion that needs to be clarified about significant
digits between tolerance/gtol and tolerance block. That clarification should
deal with the trailing zero problem. Mathematically I see no point in having
to remove the leading zero from a dimension. I think the company wants to
keep these to make sure you can see the "." in .75 by marking it with a zero
as in 0.75mm.

On the pro/e side, however badly a company may want to mangle the standard,
we need some options. The standard covers many instances where the mm vs in
are different and also different dimensional situations. Pro/e gives you
like 4 options, inch/mm/both and one other extra option of how to deal with
zeros and mm vs in.

Number 1 problem, is that the options are not really covering the
possible standard possibilities so you have to "fake" dimensions every now
and then. (I don't have an example right now and I bet its difficult to come
up with one). Numero Dos problemo is that the options in pro/e cover non
standard possibilities (to a limited extent). Use option "both" and you'll
be wrong at least half of the time :).

I propose a tolerance/dimensioning window/panel where you can set how
dimensions will be shown when you right click on a dimension to get to its
property's window. PTC can also continue to follow the standards ISO or ANSI
and have a standard.pro to set your own modifications.

And also if they added a "no economic collapse" button I would not have to
worry too much about making my drawings perfect, fast or on time. Usually
you focus on one of those tree but not all three at once.


Here is the excerpt from Terry's email in 08, see if you can come up with
a dimension that violates a standard. Maybe we can come up with a list of
if-then-else statements that PTC could use to prevent the violation of the
standard and a .pro option to allow them back.

*DRAWING SETUP OPTIONS settings*
*lead_trail_zeros*

controls the display of leading and trailing zeros in dimensions.

- *std_default**—displays only trailing zeros. no leading zeros are
displayed.
- *std_metric*—displays only leading zeros. trailing zeros are not
displayed.
- *std_english*—displays only trailing zeros. leading zeros are not
displayed.
- *both*—both leading and trailing zeros are displayed.

*note:*

- if the lead_trail_zeros_scope drawing setup option is set to all, the
lead_trail_zeros drawing setup file option controls the display of leading
and trailing zeros in dimensions, hole parameters within hole notes, and
all floating point parameters on a drawing, including parametric notes, view
scale notes, tables, symbols, and cosmetic thread notes.
- in case of dual dimensioning, the lead_trail_zeros drawing setup file
option controls the use of leading and trailing zeros in both std_english
and std_metric standards independently.
- if the units in the dual_dimensioning drawing setup file option are
primary[secondary], std_english[std_metric] shows the primary units values
with trailing zeros, while the secondary units show values with leading
zeros.
- if the units in the dual_dimensioning drawing setup file option are
secondary[primary], std_english [std_metric] secondary units show values
with trailing zeros, while the primary units show values with leading
zeros.
- hole parameters within the hole notes appear with 3 decimals,
regardless of the value set for the default_dec_places configuration option.
if you want to change the number of decimal places for the hole parameter,
type [.n] after the parameter in the text tab of the note properties dialog
box. here, n is the number of decimal places. you can edit the hole
parameter values only through the note properties dialog box that opens when
you select the hole note and click edit > value. alternatively, to edit hole
parameter values through the note properties dialog box, select the hole
note, right-click, and click edit value on the shortcut menu.
- *lead_trail_zeros_scope*

controls whether only dimensions are affected by the setting of the drawing
setup option lead_trail_zeros.

- *dims**—the drawing setup option lead_trail_zeros controls only
dimensions.
- *all—*the drawing setup option *lead_trail_zeros* controls dimensions,
hole parameters within hole notes and also all floating point parameters on
a drawing, including parametric notes, view scale notes, tables, symbols,
and cosmetic thread notes.
- *draw_ang_unit_trail_zeros*

controls display of angular dimensions.

- *yes**—removes trailing zeros (in adherence to ansi standards) when
showing angular dimensions in degrees/minutes/seconds format.
- *no*—does not display trailing zeros in angular dimensions or
tolerances.

[awright-2]

HI,

I have been battling CREO with trailing zeros and dimension tolerancing, and just about beaten it into submission for drawing dimensions, but my battle persists for the hole call outs and scale figures.

It defaults to 3 decimal places, how do I change this to 1? I tried to follow your comment below but all it kept doing was adding “.n” in the text line instead of adding a control function.

Obviously I am doing something wrong, but need pointing out what.

Reading you comment:

“- hole parameters within the hole notes appear with 3 decimals,
regardless of the value set for the default_dec_places configuration option.
if you want to change the number of decimal places for the hole parameter,
type [.n] after the parameter in the text tab of the note properties dialog
box. here, n is the number of decimal places. you can edit the hole
parameter values only through the note properties dialog box that opens when
you select the hole note and click edit > value. alternatively, to edit hole
parameter values through the note properties dialog box, select the hole
note, right-click, and click edit value on the shortcut menu.”

This is what’s displaying:

Given by the following text string:

            &METRIC_SIZE &THREAD_SERIES - &THREAD_CLASS &STD_HOLE_TYPE &VAR_THREAD &THREAD_DEPTH

DRILL  &DIAMETER THRU ONCE

My question is, do I put .n or [.n] after evey dimension I want to control the dp, or at the end of the string to control everything within that text box?

Thanks

Adam

[BenLoosli]

Replace the 'n' with a numeric value for the number of decimal places you want to show.

It truncates the display, not rounds.

rawnumber = 15.2654

&rawnumber[.3] = 15.265

&rawnumber[.2] = 15.26

&rawnumber[.1] = 15.2

[awright-2]

Thanks Ben, thats worked a treat!

How do I change the displayed decimal places on dimensions in model sketches?

Thanks

[BenLoosli]

That is done through the dimension properties dialog box.

There is a config.pro option default_dec_places that can be set to control new sketch dimension decimal places.

[awright-2]

Excellent, thanks again Ben.

[BenLoosli]

Since the process that PTC uses follows the ASME Y14.5 spec, there is no need to review it. If your company chooses to deviate from that spec, then you need to document what is different and be prepared to send that change sheet to all your suppliers and customers who receive your drawings. I will assume that your drawings have something like "Drawn IAW ASME Y14.5-YEAR" on them.

From your original post, PTC covers the leading zero on mm dimensions of less than 1.

For trailing zero to hold decimal places, why? 15.03 is the same as 15.0300, especially on a basic dimension. If someone knows the dimensioning standard convention, glancing at a drawing and seeing trailing zeros, they think the drawing is in INCHES! There is the visual presentation of the drawing to take into account when you change from what a standard specifies.


Thank you,

Ben H. Loosli
USEC, INC.