Hello Creo Experts,
I want to show only specific 10 dimensions out of 100 retrived from annotations in drawing from sketch drawn in model.
Is there any method to directly show only those specific 10 dimensions quickly out of 100s of dimension displayed in show dimension via. Annotation tab without requirement to select those 10 out of 100s of dimension.
In short I want to show only those dimension which are relevent to machining and manufacturing of drawing in shortest time. Please suggest a solution.
Thanks in advance.
I don't know how to do this but one question in my mind begs to be asked.
I am assuming (yeah, I know) that the drawing/part is being fully dimensioned
If you need only 10 dimensions to describe a part, why is there hundreds to go thru?
As a suggestion though to your troubles, in the bottom left of the Show Model Annotations window, there are two icons.
Select the right one to deselect the hundreds, then select the 10 dimensions you wish to show.
You can select either the dimension in the Annotation window or the dimension in the view.
It takes too much time to select required 10 dimensions out of 25 to 30 different ones (I have used 100 only for example) although you select only sketch feature from model tree.
So if there is any option available during sketching the geometry to highlight only those 10 dimension it would be beneficial when you have many drawings to be executed during single day.
I think what Ron was saying was don't add dimensions to your sketch feature that are not needed for machining and/or manufacturing. The software does not determine which dimension is important.
I suspect we are misunderstanding the intent of your question. Perhaps an image would help clarify.
Playing devil's advocate a little: don't create sketches that have hundreds of dimensions! I was always taught that Pro/E (sorry, Creo) worked better with many, simple features. If you create simple sketches (no more than about six dimensions) then you can easily select dimensions by feature.
Are you asking how a model can be set up to lower your workload by someone else making an effort to pre-define which dimensions are to be shown?
If so, then yes - the person making the model can place all the dimensions to be hidden on a layer so they can be blanked or selected by layer to be erased or deleted from the drawing. For extra effort, the dimensions to be kept could be named so they could be selected separately using the Find command.
There is no switch or setting in sketcher to control visibility of dimensions later.
A more general question is - since these dimensions determine the characteristics of the model, why would there be so many unimportant dimensions? If there are too many unnecessary dimensions, the best thing is to not create too many unnecessary dimensions.
Perhaps there is a picture that would show the extra dimensions and why they should not be shown.
You can select features that are machined instead of selecting views when showing dimensions.
I'm not sure I understand your question though. As Steven suggested maybe you can clarify.
I have to agree with Mark. The means to your end is to select the feature you want to display the dimensions for by view. Then only valid dimensions for that view and provided by that feature show up.
You can also erase dimensions. This hides them from future annotation selections. It is a love/hate feature of Creo.
You might be able to do something with layers but I doubt this will ever be useful or efficient.
If you ask PTC, however, they may tell you to use annotation elements. Define your full machining requirements in the model so anyone can pick this information up to create a detail drawing.
There may be many disagreements from others on this, but I'm willing to risk the firestorm. This is one of the many reasons that I advocate creating dimensions in a drawing. First, often I have found that during the course of the design process the datum structure changes. To be able to show all dimensions in this case features would have to be redefined to new references and adds to the possibility of errors being made. The only thing that you lose is that you cannot drive a dimensional change from the drawing, but if you change the model the created dimension is associative and will update unless the change you made has removed one of the items you used to create the dimension like an edge. Many people complain that this makes the created dimension turn purple but my response is that a change like that would likely have meant that the shown dimension would actually have been deleted. Personally I prefer that the purple dimension be left there to show that something happened rather than have a shown dimension simply disappear.
Let me be clear about 1 thing, I do NOT allow those created dimensions to be overridden. Only created dimensions can be overridden but that is a bad practice that should not be allowed and I stress that I don't allow it.
To be straight, Creo doesn't not know what dimensions you are interested in a feature, so you will end up seeing all the dimensions when you use Show annotations.
So there is no way (as in know with my experience) that you will be able to show only what you want.