Sketch reference to edge - Not projected geometry

[LSP-MULLERUP]

Hi

I've worked with SolidWorks for 3 years. Lots of functions and features are very alike in SW and Inventor. However some differences occur. For example:

Like in SW I select a Face on my Part and create a Sketch on it. In SW I could draw som geometry and place constraints and measuerments with respect to edges, planes, center lines and others.
In Inventor however I cannot make constraints directly to an edge. Apparently I have to project the geometry. I know this happens automaticly on Faces. But the projected geometries are "dead". So when I change a Feature I often have to fix some of the following Features because these use "dead" and "un-updated" reference geometry.

Is it possible to constrain sketch geometry directly to an edge?

Lars

[JDMather]

You may experience some frustration moving from one CAD program to another. There is a method of autoprojecting via scrubbing an edge. It isn't quite the same as the SWX technique. I suggest going through this document first http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf
and then come back and I'll explain the "scrubbing" technique in Inventor.

JD
Certified SolidWorks Professional
Autodesk Inventor Certified Expert

[LSP-MULLERUP]

Thanks for the quick reply. I'm traveling on business tomorrow so I'll look at it friday.

Lars

[LSP-MULLERUP]

Ok. I've read the paper. Very inspiring. Learned a thing or five.

So what is this "scrubbing" thing?

Lars

[SBix26]

I'm using Inventor 2008, and when I constrain or dimension sketch geometry, all edges and part features are available and automatically project to the sketch when selected. Maybe I didn't understand your question, though. Which version are you using?

[swalton]

I turned off the autoproject edges during sketch creation because I did not like the way sketches would fail when I changed the projected geometry. I wish that if I projected a surface that I got a single construction curve that would update better than the edge projection that IV uses. When I project a surface onto a sketch in ProE, I get a reference line that extends to infinity in each direction and that is always tied to that surface, even if I insert features that alter the surface before the sketch. It seems much more stable then IV. Of course thismy experience may be operator error. 😉

Feature Request: reference repair option for Skecth Doctor. This tool would allow you to select each instance of sick projected geometry and then select a replacement reference. That way you wouldn't have to delete healty portions of your sketch to clean up the sick portions.

[LSP-MULLERUP]

I may have found the answer to my own question. I found this in Inventor help:

Project geometry to the sketch plane

Project edges, vertices, work features, loops and curves from existing sketches onto the current sketch plane. You can use the projected geometry in the current sketch as a profile or path, or to constrain or dimension sketch curves or points.


In an assembly, project edges of a component cut by an assembly section view, if the uncut part intersects the sketch plane. The projected edges are not associative and will not update when the parent geometry is moved or resized.

So if I figure this right it works like this:

In a part the projected geometry will update with the geometry.

In an assembly the projected geometry in part A is "dead" and will not update if the projected geometry comes from another part.


Is this correct?

Lars

[SBix26]

I don't have autoproject edges turned on, either. I get an edge projected to my sketch when I pick it to constrain or dimesion.

I like your feature request! Can you add that to the AUGI Inventor wish list for the next cycle?

[JDMather]

I would suggest not trying to use SolidWorks techniques in Inventor and just get used to the fact that they are different.
In the classroom we actually set up each to resemble each other as much as possible but at a point you just learn to accept each for the different ways they do things. They are more alike than the are different.

You can sort of set up Inventor to Autoproject on "scrub" of an edge (see animated GIF attached), but I prefer to simply add the constraints after sketching. That technique will also autoproject the edges. And dimensioning will also autoproject edges but sometimes it can be finicky on first pick so I always pick the sketch geometry first and then the edge I want to autoproject.

[Josh_Petitt]

the key words in the phrase below are: "In an assembly"

Projecting face loops, edges and points from one part into another parts sketches is not associative and in IV is bad practice IMHO. Within a part, you can project face loops onto sketches and these are associative and very stable.

To create parts that "fit together", there are two methods that I like. The first is deriving parameters/sketches from one part into another (can be used for skeletal modelling) and adaptive parts. Adaptive parts can be a real pain, but if used correctly can be very useful.

[Anonymous]

Proper setting of Applications Options > Sketch can help in this area... see
attached.

--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
Instructor/Author/Sr. App Engr.
AIP 2008 SP2, AIP 2009 PcCillin AV
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Geforce Go 440, Driver: .8185
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http://teknigroup.com
wrote in message news:5992694@discussion.autodesk.com...
Hi

I've worked with SolidWorks for 3 years. Lots of functions and features are
very alike in SW and Inventor. However some differences occur. For example:

Like in SW I select a Face on my Part and create a Sketch on it. In SW I
could draw som geometry and place constraints and measuerments with respect
to edges, planes, center lines and others.
In Inventor however I cannot make constraints directly to an edge.
Apparently I have to project the geometry. I know this happens automaticly
on Faces. But the projected geometries are "dead". So when I change a
Feature I often have to fix some of the following Features because these use
"dead" and "un-updated" reference geometry.

Is it possible to constrain sketch geometry directly to an edge?

Lars

[Anonymous]

Hi Lars,

Scrubbing refers to moving the pointer along sketch geometry. In Inventor,
you have to scrub geometry for 3-5 mouse moves before Inventor will
recognize it. Mouse moves refer to the signal that the program gets from the
mouse. Since this is mouse movement, the distance required for scrubbing
isn't consistent.

In Inventor, the concept of scrubbing sketch geometry is pretty important.
When you are automatically applying sketch constraints, the solver will use
whatever piece of geometry it can. If you want a parallel constraint to a
particular side of a rectangle instead of a perpendicular constraint to
adjacent side, you use scrubbing to tell Inventor you want to use that line.
The reason you have to scrub in this situation is that if a touch changed
the reference, it would update each time it crossed geometry between the
line you wanted and where you need to click. Since scrubbing requires
movement along geometry, simply crossing another line won't generate enough
mouse moves to change the reference. This is one of those hidden pieces of
functionality that will help you capture design intent.

The attached AVI shows how to set a reference by scrubbing. You will notice
that Inventor still displays other constraints as they are available while I
mouse back, but once I start drawing a horizontal line it infers a parallel
constraint instead of the perpendicular constraint.

Technically, what JD shows in his animation is hovering, not scrubbing.
Hovering involves stopping the pointer over a particular spot. Once Inventor
gets a certain number of signals from the same position, it assumes that you
want to project that edge. Select Other works the same way. Since people are
very particular about how long they have to hover before Select Other
displays, there is a setting in the Application Options that controls the
delay or turns it off entirely.

Loren Jahraus
Autodesk Inventor Product Design

wrote in message news:5996205@discussion.autodesk.com...

So what is this "scrubbing" thing?

[LSP-MULLERUP]

I'm not having trouble accepting that they are different. I just know that they are so much alike that chances are that if I could do something in SW I can probably do it in IV as well. The only question is how.

Like driving two different brands of cars. The princeple in shifting gear or turning on the head light will most likely be the same. But exactly how to do it may be different.

Thanks for the advice and help.

Lars