Inventor general usability 1

[tph216]

Hi,

I have come onto using Inventor at a clients request (from Solidworks & NX), and am finding myself astounded by the shoddiness of the way in which Inventor does various things. I am here to check whether this is just me using the program wrong, or whether I am actually operating it correctly (i.e. I don't want to blame my tools if it's me who's at fault).

Now, what I have found, is that inventor almost forces me to model in a slow manner. It actually creates work for me!?

For example, when I start a sketch, I cannot dimension from the origin axes or planes. I have to first project them into the new sketch, creating new entities. Why? Why aren't these automatically directly referencable in all new sketches? Why create new redundant entities for these objects in the first place? I cannot fathom a benefit in doing it this way.

This may seem like a trivial complaint, but it means, for example, that I then have to do two time consuming things as a matter of routine:

1) Carry out the operation of creating these datums in every new sketch (i.e. turn on visibility of the master datums, "include / project geometry" for them all, turn off visibility of the master datums, use the newly created datums, then turn off visibility of the new datums each time I'm done using them, so they don't obscure the rest of my model).

2) Control the visibility of sets of datums under multiple parts, sketches and piping runs. For example, today I made the whole Tube & Piping assembly invisible, then visible again, and this turned on the visibility for all included & projected geometry). From what I can tell, I will have to go through and manually make hundreds of planes invisible now. I could turn off display of user work planes / axes, but this will also obscure any local planes or axes I may need.

This is frustrating because every single occurrence of one of those planes or axes is redundant. They are creating unproductive work for me in managing the above.

In Solidworks there is one master set of datums all referencable from any sketch or feature. There is no redundancy, and visibility is much easier to control.

It seems to me that Inventor is breaking a fundamental rule of good database design. It is encouraging the creation of duplicated entities, whilst adding no new informational content.

Why?

Am I using it wrong?

(I have further examples of terribly frustrating things in Inventor, but don't want to ramble on any more than I have to here, and am really looking for solutions rather than just to moan about Inventor).

Any help / advice would be much appreciated.

 

[rollupswx]

How much training in Inventor have you had?

http://home.pct.edu/~jmather/skillsusa university.pdf

CSWP
Autodesk Inventor Certified Expert

 

[mflayler]

Personally, I rarely find use for the Planes, the Origin CP does just about everything I need for 90% of my sketches.

There are ways to alleviate your transition, but you really need to have perhaps a one day OTS with your reseller or with a in house Inventor guru.

I have found myself astounded as shoddiness of SolidWorks in a lot of ways too, you will find there are hits and misses on both sides of the fence, but one you understand the method you get really good at avoided mis-step and increasing your productivity.

 

[mcgyvr]

tools..application options..sketch tab.. Check "autoproject part origin on sketch create" Dimension/constrain your sketches to that point..
I have NEVER dimensioned to a plane (dataum) except when I first starting playing with ProE 15 years ago before I knew any better.

 

[rollupswx]

I don't project or use the planes for dimensioning either.
Only need the origin.
Each program has it's hurdles to overcome. I have found the easiest way to do this is to sit down with someone experienced with the new program and the old to help get over the initial hurdles.
Those who go-it-alone often never get over the hurdles and instead become covinced that the new program (to them) is too flawed to even be worth their time to learn.

 

[tph216]

Did I mention I am having this problem in 3D sketches. Dimensioning to a point is fine for a 2D sketch, but for 3D you need to go to a plane in order to adequately define the direction of the dimension. If I dimensioned back to the origin point in the 3D sketch, it would do a direct point to point dimension (hypotenuse type thing).

This whole "having to project master datum geometry" thing feels to me like a major flaw in Inventor. The whole idea of those is that they never change, they are an absolute, for any given model, and so only 1 'copy' in each file should suffice. Any more are redundant.

A second example, in assembly modelling, when I place a component in a roughly right position and then begin to apply mates, the component is automatically moved by Inventor to 0,0,0. This loses any information I imparted on it when I moved it to a roughly right position. In SW, I would place the component roughly right, mate between the relevant reference plane of the component and the relevant assembly master datum plane, click distance mate, and it would leave the component where I placed it but fill in the dialogue box with the offset distance. I'd then tweak this as necessary and apply. When Inventor relocates the component to zero, it loses this useful information I imparted on the object, and slows me down.

I will give it to Inventor, that it does one or two things impressively. I was impressed by the simplicity and apparent stability in which design tables work. And the standard parts libraries look very good, as does the hole wizard & bolting. 'Frame generator' on the other hand, is terrible compared to SW's.

 

[rollupswx]

I (almost) always use 2D sketches to create and control 3D sketches. Much easier.
See Tutorial #7 Inventor or SolidWorks.

 

[EngAddict]

I also only use the origin and have it auto projected and I rarely use planes or axes. I still don't understand why SWx and ProE users complain so much about it. The 'centre point' is stored in the 'origin' folder and never moves, there is only one ever in a part or assembly file. It is only the projection of this point that is pulled through into the individual sketches, 'essentially' the exact same thing that happens when you select the origin in solidworks.
This is along the lines of SWx users asking "how can I make my work planes visible by default?". You don't need to, leave them off..
The same goes for the plane and sketch visibility you mentioned. When you modify your master part in context you remove the associativity of the file from ViewRep and you will need to set it back. Open your master part separately, make your change, Ctrl+Tab, Global Update and everything stays displayed correctly.

If you want orthogonal dimensioning in 3D space how do you know what to use as the reference plane for the dimension?.. I also use 2D sketches wherever possible and drive my 3D sketches from those. Granted Inventor could improve its 3D sketch functionality, for the amount I rely on it solely it doesn't bother me too much.

As far as your constraint complaint, you need to check the box for predict offset and orientation so it doesn't default to 0. It will stay this way until you change it.

Most of it just comes down to knowing what to look for and where to find it. Some commands that SolidWorks has but inventor doesn't have may not be a flaw, but instead isn't needed in Inventor because it handles parameters MUCH better and you can create the same effect with cleaner work flows (linked patterns as an example).

I have a user here that came from SolidWorks now he prefers Inventor and admits it is much more powerful when using master skeletal and multi-body techniques (which is all designs these days).

Both programs have their good and bad, while you can get there without training you will need to keep an open mind. Ideally though get someone into the office to ease the transition if other staff are not suitable.

 

[Blue3]

I had the same reaction when I first came to Inventor from SW. It's true what others have said that you quickly get used to the differences, but some of the defenses of Inventor seem to be more defenses of a particular way of working, as opposed to arguments that provide a rationale for why the tool works the way it does.

In general, Inventor puts a lot more restrictions on the way you can dimension and mate (constrain) than SW does. That's not a blanket criticism, there are lots of things Inventor does better (parametric modeling, for example). I think that as customers it behooves us to acknowledge the advantages and disadvantages of each product, as that's what will put pressure on the two companies to improve.

Caveat: I'm working with Inventor 2010 and SW 2010. Some things may have changed in later versions.

 

[rollupswx]

I think that as customers it behooves us to acknowledge the advantages and disadvantages of each product...

http://beta.autodesk.com

 

[tph216]

@EngAddict: I don't agree that the projection of origin points into individual sketches in Inventor is essentially the same as what SW does. Or any other origin plane or axis either.

In the underlying database of either package, when you do something like insert a dimension, you are creating a reference, e.g.

In SW, you might have something of the form:
"Dim1", distance between Point1@Sketch1 and XY-Plane@Part = 100mm.

In Inventor, this would be of the form:
"Point0@Sketch1" = CentrePoint@Part
"Dim1", distance between Point1@Sketch1 and Point0@Sketch1 in X = 100mm.

In doing that routine operation, Inventor has created an additional relationship and entity, which as far as I can tell is redundant.

E.g.
"Point0@Sketch1" is equivalent to CentrePoint@Part.
"Point0@Sketch2" is equivalent to CentrePoint@Part.
"Point0@Sketch3" is equivalent to CentrePoint@Part.
Etc...etc...

In which case, just use CentrePoint@Part directly; it will never change. In effect, Inventor is building up layers and layers of identical entities.

I suspect this may be a carry-over from the days of Autocad where layers and projections were such a common way of working.

Thinking about SW further, it is true that generally any visible geometry is selectable from a sketch for dimensioning or constraint. This includes faces / edges / points on previously created features. When you click them from a 2D sketch, SW obviously makes the projection itself, on-the-fly, as and when you need it, and keeps its control and visibility out of control of the user. I.e. It does all that for you.

The only reason I can think why Inventor may work in this way would be to improve memory / rebuild performance, where these projections are not recalculated on every rebuild. I think they probably are in SW.

I'm still not a fan of this way of working, though. It is slow; More mouse clicks, more manual layer / visibility management required, more thinking to do. I just want to concentrate on sketching / modelling, not wrestling a cumbersome unintuitive user interface.

On the other issue, I shall try the predict offset check-box, that sounds like it will do what I require.

 

[Standing]

Thank you rollupswx for the great tips. I have had Inventor training and always looking for more. A star for you.

Standing
AutoDesk Inventor Router 2011
SolidWorks Pro 2010 x64, SP5.0, SolidWorks BOM,
HP xw8600, 64-bit Windows 7
Intel Xeon CPU, 3.00 GHz, 16 GB RAM, Virtual memory 166682 MB, nVidia Quadro FX 4600

 

[splats]

tph216,

Inventor sketches do not care about default datums, the origin, or geometry projected from other features. Any references made to them (in a sketch) will be abandoned should you try to move that sketch to another surface (even a parallel surface).

What Inventor does care about, is a unique sketch coordinate system that is placed (arbitrarily?) according to the geometry of the surface that your sketch is on.

For example - if the surface for a sketch is rectangular, then Inventor will choose one of the corners for the sketch origin, and then it will orient x and y along two of the legs (I haven’t spent the time to determine how it decides which leg is which). Alternatively, if the surface you’re drawing on is circular, then the sketch origin is placed at the center of the surface.

To see what I mean, move a feature’s sketch from a rectangular surface, to a circular surface (or vice-versa). Make sure that the feature is fully constrained (use projected planes, or edges, or even the part origin). You will see that those constraints are irrelevant to Inventor and that the projected entities are no longer attached to anything.

What all of this means then, is that no matter how diligent you are in constraining features to origin of a part, Inventor will - given the opportunity - override those constraints in preference of a meaningless sketch origin.

This post may not help you cope with frustrations, but it may give you insight as to what to expect when you try to do things that every other cad system in the world - save Inventor - is able to deal with.

(I will now be told that I need more training.)

- splats -

 

[mflayler]

I have been using Inventor for 10+ years and find it very rare that I have to move a sketch in the manner you are describing on a daily basis. But what you are describing is as designed basd on the way Inventor handles projected geometry. In the end it is a little more complex for their methodolody of projection, but I still think it better than most if used correctly.

I don't think you need more training, but perhaps better best practices.

 

[rollupswx]

This post may not help you cope with frustrations...

I'm confused just reading the post.

 

[EngAddict]

It comes down to design approach and planning your model, most of the time I have it modelled in my head before I even draw a line so I rarely need to redefine a sketch.

@tph216
For a start the need to have such long winded parameters is agricultural at best. Rather than put ...@... lets just use any parameter I want directly and name it whatever I want, can argue with that.

I am not going to get back into the centre point debate, I think it has been done to death. You may have missed my point..

I'm still not a fan of this way of working, though. It is slow; More mouse clicks, more manual layer / visibility management required, more thinking to do. I just want to concentrate on sketching / modelling, not wrestling a cumbersome unintuitive user interface.

I actually think all these points are handled better in Inventor. For a start it is a fact that there are less mouse click with Inventor and the workflows are more flexible. The rest just comes down to time with the software, see if you still agree after a year or two.

 

[tph216]

I would be interested to see some design exercises in the form of races to model a range of parts, by expert users of SW and Inventor respectively.

I'm not that unfamiliar with Inventor, but I can't see SW being beat for speed and flexibility.

And just stating "it is a fact that there are fewer clicks / better workflow in Inventor doesn't make it so".

For example, starting from a new part file, to produce a model of a circular tube resting on the Top (XZ) & Right (YZ) planes, mouse clicks would be:

1. Click XY plane.
2. Click new sketch.
3. Press S & click centrepoint circle.
4. Click somewhere for the centre (not 0,0) and drag out circle to arbitrary size.
5. Click to terminate circle by radius.
6. Hold control & click on the circle.
7. Keep control held and click Right plane.
8. Let go of control & click tangent constraint.
9. Hold control & click on the circle.
10. Keep control held and click Top plane.
11. Let go of control & click tangent constraint.
12. Press S & click dimension tool.
13. Click circle.
14. Place dimension & click, then type value in box that appears.
15. Click extrude & key in an extrude length.
16. Click thin feature.
17. Key in a wall thickness & hit enter.

Then Spacebar > ISO, to get back to a nice isometric view.

Those operations could all be done in fewer than 10 seconds, by someone who knows the program well.

It is not uncommon for someone fluent in Solidworks to sit modelling on-command from other engineers or bosses, as they speak, without them having to pause and wait for the modeller to catch up (kind of in the way that a secretary might make short-hand notes at a meeting). I have never seen anyone using Inventor in that way. I have seen it in SpaceClaim, and I think CoCreate. Definitely not in Catia or NX, though.

 

[rollupswx]

I would be interested to see some design exercises in the form of races...

How much would you like to wager?

I'll wager that I can run Inventor against you running SolidWorks and beat you.

I'll wager that I can change seats with you and run SolidWorks against you running Inventor and beat you.

I'll then wager that I can run SolidWorks against you running SolidWorks and beat you again. (read it again)

 

[tph216]

I'll wager that I can run Inventor against you running SolidWorks and beat you.

Don't necessarily agree; we have no way of knowing for sure.

I'll wager that I can change seats with you and run SolidWorks against you running Inventor and beat you.

Well obviously, I'm experienced in Solidworks and out of practice in Inventor, so this follows (I won't disagree, but again have no way of knowing for sure).

I'll then wager that I can run SolidWorks against you running SolidWorks and beat you again. (read it again)

Well this isn't really what I'm comparing. Great, if you're faster than me in Solidworks (I don't really care).

How about comparing YOU running Solidworks versus YOU running Inventor, since my original question was one of comparing the software and not users, and you failed to answer this in your brilliant evaluation of how great your skills are compared against mine.

I should add that I'm not just a blind follower of Solidworks because its all I know. I specified Solidworks in my previous company after extensive investigations of a number of options (Inventor, Solidworks, SolidEdge - this was in 2006). I'd come from learning CAD on Unigraphics (v17), and using a student copy of Inventor at home, but investigated with an open mind and concluded that Solidworks was the most appropriate for our needs in my company. I would happily abandon Solidworks in a heartbeat if something better came along (may be in the process of this if SpaceClaim continues to impress & fulfil all our needs).

 

[rollupswx]

...may be in the process of this if SpaceClaim continues to impress...

LOL