Can Creo directly open a drawing from an open part?

[awright-2]

As a certified SolidWorks professional now using Creo there are a few shortcuts I miss, one of which is being able to open a drawing for a part from the model tree. In Solidworks you can do this with ether a part file or and assembly, but you can find the part in the model tree, right click and select open drawing. This shortcut will then open the drawing associated with that part without having to cycle through menus and folders looking for the drawing required.

Is this something you can do in Creo 3.0 or do I have to make a macro linked to a hot key to make this functionality?

Also, if I amend a part, should the drawing automatically update when I next open the drawing? at the moment, when I open the drawing for an amended part the dimensions all move to the new locations, but the features appear to remain in the old position. How can I refresh the drawing as the regenerate button doesn't make any difference?

Thanks

[StephenW]

You can not open a drawing directly from a part or assembly.

The drawing refresh is the chase your tails icon "UPDATE SHEETS" under the review tab or I added it to the quick toolbar.

There is an option to regen the views automatically AUTO_REGEN VIEWS YES.

By default this is turned on. Some users turn it off to speed up the system to not have the drawing regenerating views until they are told to. Its important with large assemblies and complex part models.

[awright-2]

Thanks for that, I’m only a week into using Creo 3.0 and getting used to what feels a backward, more complicated way of modelling and drawing when compared to Solidworks.

How do you add the button to the quick toolbar?

I did check and the AUTO_REGEN VIEWS is set to YES.

Thanks again

[StephenW]

Right mouse button on the quick access toolbar gives you the option to customize it.

The toolbar is mode* sensitive so items you add to the drawing quick toolbar don't add the other modes toolbar. This can be good and bad. There are a lot of modes you want to have the same options on but it does give you pretty much infinite control over what shows up in each mode.

Complicated is one way to put it. Creo (pro/e) is pretty rigid and demands attention to detail. Done right, that also means robust, rock steady models.

Drawings, well, that's never going to get better. It's obvious the attention to drawing improvements is long gone, don't hold out hope. If you do paperless (MBD), there may be hope in the future for that workflow, time will tell.

*mode as in part mode, assembly mode, sheetmetal, piping, drawing, etc.

[MikeBrattoli]

Adam,

You can also get to the Update option faster by putting your mouse over the drawing Sheet tab (normally at the bottom of the screen when the drawing is open).  Bring up your right mouse button and choose Update

[StephenW]

And welcome to the community. Good luck with the transition to Creo. I foresee headbanging in your near future. You'll need to keep an open mind!!

[BenLoosli]

You can start a savings account by tossing a quarter in a jar every time you cuss at Creo or think how much easier that function would be in SW.

Eventually you may even get a whole day without paying the jar!

Where I used to work with about 35 engineers, they bought donuts every Friday for a few months after we switched from Unigraphics V18 to Wildfire 2.

(it was one of those 'corporate' decisions that we had no say in locally. After I left, they were sold to another company and had to switch again to CATIA.)

[MartinHanak]

Hi,

see Is there a button to quickly open the drawing for an on-screen model/assembly ?

MH

[dschenken]

You may also want to shut off the option to save the display of the drawing. This particular option is the worst of the bunch. It shows the drawing mostly as it was last saved, but it updates the underlying geometry while keeping it invisible. It is supposed to be for someone who wants to see what the drawing looked like without having to regenerate all the models, but it's a landmine.

save_display Yes = makes my day bad, No = correctly display the drawing with the changes.