15-Moonstone

Question

sketcher dimension the way we want...

Forum|Forum|11 years ago
July 19, 2014
3 replies
12389 views

may be many of you know it..but i discovered this some time back...

when we give a dimension in sketcher since there is no preview..sometimes the dimension does not come the

way we want it...

for e.g.

sometimes it gives a slanted dimension instead of a vertical or horizontal dimension..because we have not clicked ideally..

so people in Pro/E 5.0 and above if you want a horizontal dimension..select the horizontal centerline after selecting the dimension points.

same is the case with vertical dimension(select a vertical centerline)

and the same for a slanted center dimension (a slanted center line)

i was not able to produce the same result in Pro/E 4.0

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2D Drawing

T

TomD.inPDX

17-Peridot

I knew about the "about the centerline" dimensions (which now automatically become diameters!) but I just relearned about "arc length". That has become -very- useful.

By the way, a centerline dim that fails to go to diameter can be changed after it is set by using the RMB and select "convert to diameter".

R

rohit_rajan

Author

15-Moonstone

yes just tried the diameter conversion one...

T

TomD.inPDX

17-Peridot

Even better, in Creo 2, if you create a datum centerline in the sketch before the geometry in a revolve, Sketcher will autogenerate diameter dimensions.

L

lroose

1-Visitor

I agree with many in this thread that IM is more of a hindrance than a help. Creo should not try to do anything for me. Just give me the tools to do what I want. For example, enable me to add constraints on the fly with the RMB menu or just highlight the constraint options when I move my mouse cursor near other geometry and let me pick one if I want it. Just don't make constraints and dimensions automatically.

This issue is similar to the one with the so-called Smart Selection Filter and pre-selection highlighting. PTC presumes to make suggestions regarding what I want to pick. KISS should dictate that only the item nearest the user gets highlighted and the user can choose whether to dig deeper with RMB clicks.

The usefulness of both the IM and SSF/pre-selection highlighting degrades quickly with increasing design complexity.

Put control in the hands of the user where it belongs. Taking it away allows poor modeling practices to propagate and makes life difficult for those attempting to create a solid design.

Patriot_1776

22-Sapphire II

Well Lee, if you'd used the old pre-WF sketcher where you had to manually do everything, you'd probably not say that. I think the best thing, would be to have the option to turn it off, and then MANUALLY constrain everything, like AutoCAD. For simple sketches, let the software do it, for complex sketches like Antonius and I like to use, let us do it manually. Oh, and we should be able to import complex sketches (like a DXF from AutoCAD) like a logo as a scaleable "block", without the IM going crazy and trying to constrain everything.

T

TomD.inPDX

17-Peridot

A paper weight on the shift key helps

S

spete

10-Marble

Keeping your sketches simple and increasing the number of features would probably alleviate some of your issues with the IM. If you must use complex sketches, then turn it off.

I tend to design parts based on how I imagine it will be fabricated. This keeps individual features simple with multiple features.

B

banderson-2

1-Visitor

I know that this is an old thread, but I am coming up on the same issue. I have a fairly involved side sheet that I have cutouts to mount the parts to. I have created the geometry in multiple sketches and extrudes to keep the sketches more simple. But now I want to use this geometry (what's highlighted in red) on a new side sheet for a slightly different application. I tried making a sketch and projecting the edges, then copying the sketch elements to a sketch to use in my pallet tool. When I do that, creo dimensions every point, and not so intelligently (see pics below), and the sketch lines don't line up at the end points, so it's an open sketch. If I start trying to constrain stuff intelligently, the lines end up moving. I'm better off just redrawing the features from scratch and using the original model as something I can measure off of or refer to the individual sketches. Blocks would be awesome in this case. What I'll probably end up doing is copying this part out and seeing if I can modify the base structure to what I need. How would you guys handle this situation?

Part I want to get info from.

what the copied sketch looks like, (after I tried to sort out some of the stuff)

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StephenW

23-Emerald III

What I would do is assemble the 2 parts together in an assembly positioned such that the cut is where I want it and then project the edges. Then, one at a time, I would remove the references to the other part and dimension as I needed it to be dimensioned. I would also break up the large feature in to smaller functional features.

The sketch you are making will work, but you have to remove all the references to anything except centerlines or construction lines contained in your sketch. References to your part will be lost when you pull it in to another part.

You can also copy-paste features. I've had some success with that too.

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