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What are the implications of using the “set independent” option?


What are the implications of using the “set independent” option?

What exactly are the implications of using the “set independent” option for external references? Does is mean that once the links are set to dependent that everything updates and you might not know what all is changed?


Mike, can you explain where you are setting this option?

You can go "edit definition" on each feature and set it to independent.

This is not the case of native features so you are talking about specific features that inherit data from external sources. When you can set them to independent, yes, you break the link but when you make them dependent, the part updates if the master is updated.

Some features don't allow independence.

The ramifications are no different on what due-diligence requires. I work very hard not to create outside dependencies. If you think about it, drawings are highly dependent on the drawing models. A change in the model can wreak havoc on the drawing. I did a simple replacement of a chamfer with a revolve cut to manage the angle better (odd interface). Since one of the surfaces was a primary datum, the whole drawing went to heck in a handbasket forcing me to re-place 2 dozen dimensions.

In addition to what Antonius has mentioned, be aware that a model may be use din MANY dwgs, so a "shown" (driving) dimension change will affect EVERY dwg it's shown in. More and more reason why I'm getting to like and use dims created at the dwg level.

That's only because you don't have malignant uses like setting a part to 9.49999 inches, and creating a dim on the drawing that is Rounded to 0 places -> 9. then having inspection complain the parts made based on the model are too long.

On projects with dozens of users of various levels of creativity, I wish PTC never allowed either creating dimensions or over-riding the text of those created dimensions.

I suspect created dimensions are also A.D.'s root problem, as created dimensions tend to reference edges, which will change, rather than faces which won't. One could create a datum plane or datum curve coincident with the face and use them as references to created dimensions. That's more work then just using the model dimensions straight-away.

I have no doubt about that, David. I will use driving dimensions when they are correctly defined in the model, but all too often, that is not the case. I look at my model in one way, and often, by the time I get to my drawing, I have to implement design intent in a different way. I find there is risk in re-defining the model just to suit the dimension on a drawing.

However, I do deploy another strategy that would work except that it is a check function. I re-model the part based on the drawing to check for completeness. I can model some pretty complex stuff in less than a half hour. Once I overlay the two, and I know all the dimensions are on the drawing, this new model would easily create a fully driving dimension drawing.

But I do use the radius dimension for nefarious reasons... things like note leaders that I want to follow the arc or "FULL R@O". So I do like the ability to overwrite dims.

Rounding dimensions I fully agree! NO ROUNDING ALLOWED! That model you give to the machinist had better be exact to the drawing. The only except is limit dimensions. I do not want limit dimensions driving nominals on the feature. A plus nothing, minus something means just that even in limit dimensions.

"I suspect created dimensions are also A.D.'s root problem, as created dimensions tend to reference edges, which will change, rather than faces which won't."

Which is why I have and recommend setting "prehighlight" to off, and using the old school "query-select" to make sure you know EXACTLY what references you're picking, for drawing use as well as ALL modeling use.

As far as rounding, do we REALLY need to go all the way out to .265625 just to get 17/64?

... no, we have to manually enter the fraction

Hah! Ok. I like the way you can actually enter17/64 and have it turn decimal in the model but we only go to 3 places for everything inch.

DWG > 17/64@O

Oops! What I meant was that if you measure something with a tape measure, and don't have the conversion chart handy, you can just type 17/64 in your sketch and it will automatically do the math and convert to .265625. I think that's pretty cool that you can do math like then when entering a number.

Did they change the syntax in creo 2? For me it's "@O17/64" to get a text string instead of numeric.

You can enter it either way. I've gotten into the habit of putting it before.

One thing I noticed in Creo 1.0 that really got my goat... And I am not certain -when- it happens.

You enter a fraction that goes out many decimal places and the entry would truncate. When you later edited the value, it would only be 3 digits. That pretty much stopped me trusting the system to what is right. I haven't seen this behavour in Creo 2.0 but I am not lookinng for it either.

Early, I was implimenting model changes and move the existing model to the side and bringing in another model into a drawing. As I dimensions the new model I deleted them off the old model (not erased, but deleted) little did I realized that I was deleting them off 50 other drawings.

Thanks, Dale

I think those would have been dimensions created in the drawing, but stored in the model and then shown on other drawings. Yup. That could cause a suprising amount of unwelcome change.


It doesn't seem possible to delete a model dimension from a drawing and have it affect other drawings, because model dimensions can't be deleted from the model, recognizing that features can be deleted and redefined, which may involve deleting related dimensions.

In a dwg you can't delete model dimensions (have to do it in the sketch), but you can MODIFY them, and add text, such as "2X" in front of a dimension, and that WILL show in the other dwgs. Also, you can change or even delete GTOLS....and that will affect other dwgs.

Caveat emptor.....

I've used the set independent option to resolve failures from copy geometry that would otherwise make a model explode.

For instance:

  • Say I have a copy geometry of some surfaces on a skeleton model of an aircraft wing. The copy geometry drives the major surfaces of a bracket that I'm working on.
  • Now, another user modifies the skeleton in a way such that my copy geometry references are blown away yet the part hasn't changed much. Now I can't regenerate my part without the model exploding.
  • So, I erase the skeleton from session and then set my copy geometry reference to independent.
  • My part will regenerate and I'm free to create a new (dependent) copy geometry reference to replace the old independent one without the entirety of my model going into an epileptic fit.
  • Now that the copy geometry is replaced with correct references that are dependent, it will always update to the latest skeleton changes.

Eric, this sooooo deserves a document of its own

Hi Eric,

Am I following right?

A) Base Model -> Copy Geom -> Skeleton Part -> Copy Geom -> Bracket.

B) Skeleton damaged by other user.

C) Bracket can be retrieved, but not Regen'ed

D) Erase Skeleton Part

E) Set Part Copy Geom References to Independent

F) Retrieve Skeleton Part

F) In Bracket, Create new, dependent References to Skeleton Part

G) Reroute Bracket references to new, dependent references

H) In Bracket, Delete old, independent Copy Geom

Is it that the skeleton is broken or is that the Base Model changed so that the skeleton is broken? Then when the skeleton is fixed, it has new references that appear coincident with the old ones.

You, sir, are correct. Good synopsis.

"G" above was a reroute in the sense that I redefined the bracket to solidify-cut to the new reference, I didn't actually perform a reroute on it...I suppose I could but poking myself in the eye would have been more fun.

Skeleton wasn't broken, just that there was a small design change and the sketch in the VSS had entities that were deleted/recreated...other user didn't use the "replace reference" option in the sketch.

Consequently my model went into an epileptic fit since basically the first feature which drives all of the datums that my model is built off of has failed. If I try to redefine in this state, I might as well start from scratch since I have to suppress everything to fix it....(it's hard to see what you are doing when everything is suppressed). To add insult to injury, the "Make independent" option in the resolve failure dialog won't work if the skeleton is in session....a day late and a dollar short. So I erased everything out of session (including the skeleton...this is important) and then changed the copy geom to be independent by redefining the copy geom in my part. Quite simple:


Now the bracket can coexist with the modified skeleton without exploding and I am free to modify what I need to and still see what I'm doing.....create a new copy geom (along with surface trims to keep things local) as a last feature in my bracket and then drag it to the beginning or desired location of the tree with it's trims.

The good: Copy geom can be used to work in very large assemblies faster. For instance if packaging/designing components on a large complex panel that takes 45 min to regen, we copy the mating surfaces and set to independent so the file opens in a couple seconds and has the required geometry to complete a design. Now the bad: We are using Creo 2.0  M130 and the set to independent works for a while then it ignores the independent check box and goes fully dependent.  Evidently there is a bug because all my independent copy geoms are pulling in the large models in the background. The tools-reference viewer shows a live link too even though the dependency box is unchecked. So I would not use the copy geom and expect "independent" option to work reliably. I have not tried Creo 3.0.

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