Adding Constraints to Sketches in Detail Drawings

[jwickham-2]

I have a few basic (I think) questions - A part on which I am working requires a certain area to be left with an as-machined finish while the rest is brushed. On the detail drawing I am trying to add a dashed line parallel to the part to indicate the as-machined region. However:

1. While I can sketch a line on the drawing, I cannot find a way to add constraints to make the sketched line parallel to the part.
2. Furthermore, when I try to dimension from the part to the line, the dimensions are driven. Thus there is no direct way to control the length of the line. Even if I get it close to the right length by dragging the ends of the line around, the dimension displays the exact value for the line length, not the exact value I want. It will not let me override the dimension to display the value I want.
3. I would also like a way to dimension from the part to the line to lock it in the right position with respect to the view, but then hide the dimension so that it does not show up on the drawing.

Any tips on how to do these things?

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[TomD.inPDX · Accepted solution]

It is a common requirement and sketching sure does leave a lot to be desired. Sketching on a drawing should be similar to sketching in a section/sketch of the model, but that is not how it is. I often find myself translating and copying, and trimming to fixed lengths. Worst case, use a grid. None of this seems very productive. Yet, I have managed extensive diagrams this way.

I think the developers are more in favor of using cosmetic sketches in the model to be turned on by layers in the drawing. These -can- be used to create drafting sketches or create hatch patterns as needed. As a matter of fact, if doesn't even have to be a cosmetic sketch. You can just make a model sketch and do the same thing.

[JonathanHodgson]

Antonius Dirriwachter wrote:

It is a common requirement and sketching sure does leave a lot to be desired.

<snip>

I think the developers are more in favor of using cosmetic sketches in the model to be turned on by layers in the drawing. These -can- be used to create drafting sketches or create hatch patterns as needed. As a matter of fact, if doesn't even have to be a cosmetic sketch. You can just make a model sketch and do the same thing.

Yup, I'd agree that the sketching tools in the drawing environment are useless, especially compared to the mode sketcher.

I've moved to placing these sketches in the model, as Antonius describes, for all but the very simplest of drawing additions. It's far more robust and allows access to all the parametric constraints and dimensions we're used to.

Just put each sketch you create on its own layer, so that you can enable them individually in the drawing.

[John.Pryal]

Hi Jeff, there are a couple of tools that might be of use to you. Try parametric sketching, here, the system remembers parametic sketch references, so addressing point number 1. Try "relate to view" to address point 3. I am not sure what version you are using, but in Creo/Elements 5, this can be found under 'Edit, Relate, Relate to View'.

Hope this helps

John

[dcox-2]

Jeff,

You can do the first thing on your list but that's about it. When sketching the line you first need to select snapping references, in this case choose a line on the drawing that you want to use as the parallel ref. The parallel constraint should be added automatically once you sketch the line close to parallel with the ref.

The other two, you're probably out of luck unfortunately; you can use 'relate to view' to lock it to the view, but without being able to create a driving dimension to position it accurately, there's not too much point in that.

I will add my voice to those above, the best thing to do is to forget about trying to do any sort of accurate sketching in the drawing environment and use cosmetic sketches in the model. Every time a new version of ProE/Creo has been released, I've hoped for some development of the drawing environment but a lot of the deep issues are still there.

I have heard suggestions that this may be because PTC believe the future of engineering doesn't include drawings and that all you need is a well sorted model. That may be so - I have nothing to back that up with, but until then I guess we just have to live with it.

[Hongjie]

I met same problem to sketch a line parallel to model edge in detail drawing, so I search the thread.

It is my luck, I find a solution, after do all you mentioned sanapping reference, you clike the reference edage(shown line), the edage two ends will show a small circle, so you can use it as star end to draft (create  ) perpendicular line, the line length is offset (distance of my expected line to reference model edge), then you continue use other end of the perpedicular line to create my expected line, which is parallel to modle edge. then you del the perpendicular line, group new parallel line to the view.

The solution is very non efficent, for only a few line create is still acceptable. It just like walk from one  corner to other corner, you need one step by one step, NOT Jump.

I use Creo 2.0

_Hongjie

[jwickham-2]

I just tried the model sketches combined with using layers - what a relief! That gets me where I need to go. Of course it would be more convenient to work directly on the detail drawing, but it is a way to at least get the information on the drawing. Thank you to all who provided advice!

[mpeterson]

And when you create these curves or surfaces in the model instead of the drawing then they are not dumb drawing sketches and will be parametric too. I create surface copies a lot to indicate on parts and drawings the different areas of texture, etc.