I'm on the prowl again for content. I need to do another user group presentation on advanced tips. I've got a bit of stuff already, but as usual, mining the newsgroup always turns up some gems that I hadn't thought of.
Examples might be like this...
- simplified configuration thingy in the open dialog
- advanced select
- cap ends in thin feature
- "thickness" link value
... and stuff like that (can't give away all my good stuff right away!)
Anyway, please chime in with obscure stuff that we've forgotten or never knew before (where's Mike Wilson when you need him?)
One pretty obscure thing that springs to mind is the way "Zoom to Selection" interacts with "Rotate about Screen Centre". Obviously "Zoom to Selection" moves the model in the display's 2D world to centre the selection. It's not so obvious that it also moves the 'z depth' of the centre of rotation to the centre of the selection. Subsequent rotation of the view will keep the selection centred, even when it is no longer selected. The beauty of using "Zoom to Selection" is that the resulting rotation-centre z-axis relocation is reverted to after you temporarily redefine the rotation centre using the "Rotate View" mouse click.
Proviso: DON'T zoom out using "Zoom to Fit": this works like "Zoom to Selection" where the selection is the whole model, consequently it moves the 'z depth' of the centre of rotation to the centre of the model. Any other zoom-out method leaves the 'z depth' location intact, so does panning.
When I got my brain around this, I found it made working alternately between two places (say two ends of a long loft) a whole lot easier.
Of course don't forget the advanced selection options in an assembly. I use them for various things like hiding all but hardware or vice versa. It actually seems to be a kind of sql type database thing.
In addition the envelope part in it's original role as a selection device and in the many other roles it can play in constructing a complex assembly.
You could probably spent a whole session opening up these two items.
OK, I'll take your challenge. How about this? When inserting a Feature (like an Extruded Cut) in an assembly one can define which components the Feature will apply to, but only AFTER creating the Feature (right-click, Feature Scope).
Perhaps ...... several traps with diameter dimensions. Most people know about the dangers of dimensioning sketch entities to construction geometry, because a single class of entity serves double duty, as construction lines and as centrelines. When combined with the "intelligent toggle" re placement of diameter dimensions, we have a potential for screwups. In the case where the dimension is small, the "toggle jump" is so small as to be easily missed. I try to be zoomed in close and/or watching carefully, in case I inadvertantly pull the arrow too far past the line and unbeknownst set up a diameter dimension in a case where there is no diameter to dimension. Another strategy is to leave the lines as solid, until all dimensions have been placed.
A more obscure and quite different trap relates to drawings, when you manually place a dimension for the diameter of a hole in a section view (where the axis of the hole lies on the section plane) by clicking on each cut edge in turn.
If there is a problem with the position of the centreplane, either accidentally or because you've offset it 0.01 to work around the PITA "invalid section" disfunctionality and subsequently forgotten about it, the displayed diameter dimension will be slightly wrong (especially for a small hole). If you're modelling precise machined parts, this may not be evident, because the desired size may not be a nice round number.
A symptom is that the diameter symbol will not come up.
A safer option is to dimension such holes within an end-on view, then drag the resulting dimension to the section view.
A slightly related trap from an entirely different cause, also in 2D drawings, is the "true" vs "projected" toggle - if it is inadvertantly set wrong, manually placed dimensions on orthographic views can tell lies if the entities are a different z-depths.
How about pointing out the obvious? A lot of the time you don't have to open the measure box to find out how long a line is, or what the distance is between 2 objects, or something. Look down at the status bar - most of the time the required info is there. Unfortunately it doesn't show the diameter of a circular object, such as the diameter of a piece of shafting, but it will show it if you pick the edge.
Or another. If you have your drawings set up "properly", then you have the title block tied to custom properties. If a user isn't thinking, or doesn't know about it, they will sometimes go into those notes, double-click, and type in their new value. This, of course, deletes the property link, never to update again.
So, it really helps if you go to the View menu and check Annotation Link Variables. With that checked, any time the user gets into a note that is tied to a property, the link shows up, and just maybe, they will realize how it's set up and not destroy it.
When doing lofts, and the profiles are circular. SW seems to determine the connection points between the profiles in an arbitrary manner. This can result in a hourglassing effect between them. When given the option, SWx will snap the connect points to sketch points so this is not an issue with other profile types.
To correct this either:
1- use the split entities funtion on the profile's circles ( must split at least two places ) and constrain the points to known entities. SWx will then connect the loft sections at these points resulting in a true circular cross section at any point along the centerline.
2- if possible, use semi-circular profiles and mirror the result
When working with imported geometry like a part used to make a cavity, name the faces used to create other features in the mold. Then when a change comes along you can name the faces on the changed part the same as the original and most of the feautures in the cavity with ties to the part surface will still work.
Wow!!! Never paid much attention to that. Good tip. Can't wait to blow my co-workers mind by telling him how long something is without opening the measure dialog.
This qualifies as obscure for sure. I knew you'd be good for some stuff like this. I've never used this function before. Do you use this on real jobs? Does the number of named faces sometimes become prohibitive or is there some way to mass select and mass name faces? Do you need to worry about the settings in Tools, Options, External References (Automatically generate names for referenced geometry)?
I know there was a thread about this recently concerning incontext. I guess I'm curious about if you actually use this or if it's just an academic possibility.
Yes, I love the overlooked obvious nuggets, especially when you can tie them into something else. That's also rather newish which may account for people not being too familiar with it.
Advanced show hide, right. Also a good reason to fill in your custom properties as you build parts as much as possible.
Remind me of the other functions of the envelope. I remember that it's a part that won't show in the bom, that you can use it as a skeleton to build from and mate to. What are the other uses?
Great, we've got some good ideas flowing here. Here's some more:
- select faces to do a partial export. when the save begins, it will ask if you are trying to save the part or just the faces.
- draw a line lined up with (starting to one side and finishing further to that side) an endpoint or the origin and it will pick up a coincident relation
- in the Bodies folders, features that affect each body are listed under the body.
- all of the "select" options from the RMB for edges, such as tangency, loop, open loop, partial loop, the inside loop trick with a face and an inside edge, also the window select options, left vs right drag window select, the new invert selection, the obvious selection filters, the Tools, Options setting that allows you to select edges through a solid model, and the seemingly undocumented fact that in SW05 this function is turned on by default by the fillet feature (although this might be a bug rather than obscure minutia).
And in the same vein you can add export faces to temp.iges, fix, delete and reimport repaired faces.
In a different vein entirely, and you could do several presentations on this, editing the special files for things like custom properties, templates, sheet formats, gtol.sym, bend tables, linetypes etc.
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