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...
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
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".
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.
Good. Now they can get cracking on the curvture element and dimension so you can go from +radius, to straight, to -radius with the same curve element.
My real problem with sketcher is constraints. When the solver finds a conflict, it does not report -all- the conflicts for selection. Sometimes very obvious conflicting dimensions are not available for selection. This has only gotten worse as Creo development goes forward.
Agree. Before Intent Manager (IM), Sketcher left one to think through how the sketch was to work. Then IM became permanent and instead of figuring out how the sketch should work, I end up trying to figure out which constraints need to be eliminated so the correct ones can be used. And when I delete one, IM jumps in a 'fixes' it for me. Like Clippy the Mime. I hate Clippy and am not that fond of Mimes.
Remembering how constraints function is one thing. Having to also remember how software will choose which constraints to apply based on the current condition of the sketch is entirely more difficult.
Here's example games:
1) Pick two numbers that add to 100.
2) Pick a number that added to the number I'm thinking of will result in 100.
Game 1 is the original Sketcher. Game 2 is Intent Manager. Guess which is won more easily.
Ever had a sketch that can't easily be changed because IM performed a common-horizontal alignment between a vertex on one side of the screen and a point on the far side of the screen? I get those and wonder how can that vertex be located when there is no dimension for it? I didn't align it, IM noticed it was close and snapped the constraint on it without asking.
I've had a lot of what I call "Intent Manager Rage" incidents. A few of the things that continually cause me grief:
(1) The sociopathic need it seems to have to make the length of whatever line I'm drawing be the same as some other line on the sketch. I am constantly forced to make randomly long lines in my sketches to avoid the manager snapping them to an undesired length.
(2) Sneaky parallelism or perpendicularity constraints being applied. Often the line it's paired up with is nowhere near and I have to play detective to determine the cause of the trouble.
(3) If I make a geometry change that disconnects a sketch curve with the edge I used to "project" it, the intent manager inserts dimensions (weak ones) to fulfill its needs, but I don't know about it. This inevitably leads to trouble for me when I make subtle changes to, for example, a width, and it "looks" good, but isn't mathematically correct.
I resisted use of the intent manager for years and years until it was forced upon me. Now, I spend time trying to anticipate what screwy behavior it is going to pull, so I can avoid it.
You guys know that you can use RMB while sketching to disable (or to lock, either with Ctrl or by cycling) each constraint that is suggested on-the-fly, right? If there are several, Tab cycles round them.
If a constraint pops up that you don't want, just disable it. If one is suggested that you do want, lock it and the current sketch element is partially constrained even before you've finished placing it.
Of course, IM was there when I started with Pro/E so I've never had the pleasure of having to assign each and evey constraint manually...
The IM is manageable, yes. Also the shift key works to disable the IM on the fly.
My biggest beef with it is the fact that I can -knowingly- have an extra locked dimension in the sketch and I want to select it when the IM kicks in. But Lo, it is not one of the listed conflicts. So I have undo the action, manually delete the interfering dimension, and then do the action again. That is a huge waste of mouseclicks.
The second, absolutely no excuse error is where the IM doesn't allow a zero degree angle on a line that is trying to square up a sketch. No matter what you do, the line won't go horizontal with the angle dimension driving it. But what do you know, a 90 degree dimensions works without issue. Once you experience this, you know this is not a robust sketch. But the reason for it is absolutely superfluous. There is a similar issue that causes all kinds failures in patterns and other things. It is a deep seated bug that really makes Creo so difficult to use.
The thing is/was it takes about the same effort to put the ones on you want, because you know what you want, as it does to find/understand/remove/avoid the ones IM assumes incorrectly. It's easier to do what you want than to avoid what you don't.
IM users can skip knowing how to get a sketch to work correctly before they can move on. It avoids frustrating users because a sketch can never fail, but it interferes with users understanding how sketches work.
Creation of parametric models is a form of software development. What IM does is the equivalent of a conventional programming language making corrections for syntax errors so the code compiles, but without ensuring the program is correct. Example: a missing a ")" ? - just add one to the end of the expression. This auto-correct makes conventional programming much harder to debug. Excel does this and it rarely gets it right, but it's part of an error message that emphasizes that a guess is being made and the program won't proceed until the error is dealt with or the correction is accepted. PTC just slips in the correction without comment.
Just the thought of going back to the pre-IM days are enough to make me cringe a little. I was one of those guys who held out a couple of releases before I accepted intent manager as a good thing. I was concerned with it dumbing down my sketches and assuming something I didn't want it to assume.
I still occassionally have a difficult time trouble-shooting some assumption that is not letting me add the dimension or constraint I want. BUT remembering back to the alternative and having to regenerate the sketch and sometimes having to zoom in to an area because regeneration of the sketches was zoom sensitive sort of like accuracy. That is exactly where KISS (Keep It Simple Stupid) principle came from. The general rule as no more than 8-10 entities in a sketch otherwise you may never get it to regenerate.
I do not have found memories of pre-IM days. I used it for several years and don't wish that evil on anyone.
Don't forget these little pearls in option settings...
These should be available inside sketcher with quick access.
I for one love to create very complex and comprehensive sketches. I find very little value in IM. An IM on/off toggle would be perfect for me.
Like you I started pre-IM. It's how I learned to do sketching well.
I just observe the results of those who either didn't learn or who started post-IM and the level and complexity of errors they allow IM to make is amazing, and can be very difficult to figure out as I don't know what they had in mind and didn't have to make a model that represented what they had in mind.
I do recall the zooming - usually to handle entities at slight angles. While one could draw the sketch in an exaggerated way, after applying the correct dimensions, on regen it would try to override the angle value (say 89.9 degrees) with a vertical constraint. It decided if the line should be vertical (or horizontal) based on the delta in screen coordinates. Since zooming would make the delta-X in screen coordinates larger, it would decrease the chance of being detected as a vertical line. On the other hand, if there was a mismatch in the sketch where line ends weren't drawn coincident, zooming up would prevent them from being seen as coincident and would fail the sketch as they had insufficient dimensions. It was sometimes a balance between zoom in and zoom out to get the desired result.
For those using IM, the original Sketcher did not have tools to force vertical or horizontal constraints. I think I would have used a grid if there was one.
The solution I considered was a false-sketch process, where the sketch regen would decide if the sketch could be regenerated, but the sketch geometry would not be moved. This way a line could be drawn at, say 75 degrees and dimensioned to be 89.9 degrees. If the constraints were sufficient, then OK, and Sketcher would create the correct geometry output required, which would be at 89.9 degrees, but in Sketcher it would still be at 75 degrees, so the slope was obvious. If the user cared to, I suppose a 'clean-up' button could substitute the correct geometry. This is similar to how people understand a hand sketch. It doesn't have to be micron level perfect to build a micron level part.
Instead it was possible to create a sketch that could easily regenerate and produce a resulting sketch that would not easily regenerate.
Unless I'm misremembering, all assumed constraints are grey (weak), right? We just set a rule that you do not leave a sketch with weak dimensions or constraints.
I like the fact that IM effectively regenerates dynamically; admittedly you occasionally have to trick it if you want to change a sketch substantially, but for the most part you know that it's working as you create it. Just once in a blue moon I'll use the 'change dimensions' tool and un-tick the auto-regenerate checkbox.
To each their own, but I've never felt the need to disable IM since I first learnt on 2000i^2...
You can "set a rule" that you don't leave weak constraints in sketches, but that does nothing to prevent Creo from putting them in for you, without telling you, when it feels the need. As I said earlier, I've had instances where geometry that was "projected" in a sketch has become detached for some reason. Creo sees this and puts a weak dimension in, saving me the "bother" of adhering to my design intent. Thereafter, when I make changes to the geometry that I intended to be the driver of the model, the weakly dimensioned features do not follow along. Non-hilarity ensues.
The problem, even with weak constraints and dimensions, is that they do on occasion prevent you from dragging the sketch to where you want it. And you cannot delete them! You can only replace them with a strong replacement as a placeholder.
I also lock all edited and placed dimensions. This lets me sneak up on the IM one piece at a time. For every 2 dimensions or constraints I place, I have to delete one or redo one. Pretty poor odds.
There's an auto-regenerate checkbox?
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.
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.
Blocks would be nice. There are times I am just interested in copying something without changing it, except for its position.
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.
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)
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.