Create Drawing Dims option

[gkemner]

I am trying to get an understanding of the Pros/Cons for this config
option:

create_drawing_dims_only

The default is "NO" which means that dims created in the drawing are
actually stored in the model. If you are using Intralink/PDMlink that
then means that to create a driven dimension in the drawing the part or
assembly model will also be marked as modified and have to be checked
out along with the drawing. That can pose a problem in some cases. An
example would be that you are creating an envelope or spec drawing of a
part or assembly that is already releases.

If set to "YES" then dims created in the drawing are stored only in the
drawing, so only the drawing is marked as changed and the model does not
have to be check out.

We have always used the default "NO" value in the past but it now seems
to make more sense to set it to "YES" if you are using any sort of data
management tool in order to minimize the number of items that get
modified.

Any insight regarding how you have this option set and any pros/cons
would be helpful.

Thanks!

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[iturner]

Greg

I had the same problem a few years ago and I couldn't find any info on
the downsides of setting the option to yes. So we tested - no problems
and it has been that way for 3yrs and no issues. In fact it fixed a lot
of issues with Intralink.

We often had a problem (with the setting on 'no') when users would
remove read only from the drawing doe some mods , save open the drawing
again and the mods would disappear.


Ian Turner

CAD Manager

Cobham Mission Equipment

[dgschaefer]

Setting it to 'YES' will restrict the use of dimensions in notes and
other dimensions. For example, you and a hole not to contain the c'bore
diameter and dept, so you grab the dim symbols and add them using &dXX
to the through hole diameter call out. You will not be able to do that
when the option is set to 'YES'. This may only apply to using created
dims in shown and the reverse, but I don't believe so. I haven't
thoroughly tested it to find out.

This is why we've not used that setting here.

Doug Schaefer

[ptc-46674]

I have always kept the setting to NO.

If we are revising the drawing we generally want the part & or assembly to keep the same revision.

When it is set to YES, you can change the revision of the drawing without changing the revision of the part, but that get confusing what revision are we supposed to be ordering ?

keep it the same and there is no questions.

Dave McClinton

McKesson Automation

[MikeFoster]

There are two types of created dimensions that I know of. Their symbols
are, for example, ad23 and add23 (shown dims are seen as d23).



adxx dims are created when "create_drawing_dims_only" is set to "no"

addxx dims are created when "create_drawing_dims_only" is set to "yes"



It used to be that addxx dims could not be moved into notes using the
syntax &addxx and adxx dims could. For that reason we kept that config
setting to "no".



This no longer seems to be the case (WF3M160) based on a very quick
test. I therefore intend to change that setting to "yes".



Does anyone know of any other reduced functionality issues with "addxx"
type dimensions?



Thanks,



Mike Foster

ATK

[jflores-3]

Not sure but I think there was a problem attaching Gtols to the
dimensions depending on the config setting.



Thank you, Jim Flores

Mech. designer/CAD admin.

Clinical Care Systems

Philips Healthcare

2271 Cosmos Court

Carlsbad, CA. 92011

-

[MikeFoster]

Jim is correct, I confirmed that "addxx" type dimensions do indeed still
suffer from reduced functionality in that gtols cannot be attached to
them. We will therefore leave our config setting as
"create_drawing_dims_only no".



I checked this in WF3M160, anyone know if this has changed in a more
recent build of release?



Thanks,



Mike Foster

ATK

[dgallup]

While there are restrictions on what can be done with dimensions created in the drawing, there are simple work arounds that become second nature when you use the 'YES" setting. For instance, you can attach GTOLS to them but the GTOL also has to be created "in the drawing". These GTOLS can still reference model datums.

One HUGE advantage to using the "YES" setting is working with customer models. If you spend a lot of time detailing a drawing of a model that is produced offsite and save your dimensions with the model you are up the creek when you receive a new version of the model, all that detailing is gone, gone, gone.

We have used YES since the dawn of Pro/DETAIL and I would never change.

We use the model revision parameter in the drawing title block so a drawing revision change always revs the model.