Copy/Paste Problem

[JohnnyKash]

I'm having trouble getting copy/paste to work correctly in the attached file. For some reason it's pasting the sketch lines onto the other side of the disk on the third cloning. Why did it work fine on the first two?

[SBix26]

The sketch coordinate system on that third sketch is upside down compared to the first two.  Before copying the sketch geometry, you could right click on the sketch and Edit Coordinate System to set it like the other two.  But I'll also tell you that I almost never look at or care how the sketch coordinate system is oriented.  

It looks like (in JD's words) you're doing way too much work, you're not using the origin point and planes effectively, your sketches are not constrained, etc.

Have you had any training?  You might start by checking out JD's basic tutorial here.

And, if you tell or show us what you're trying to accomplish we might be able to point you in a more efficient direction; there are usually several ways to do something "right", and even more ways to do it wrong.

[JohnnyKash]

I'm trying to model Fig. 2 from this patent: http://www.google.com/patents/US7971505

[SBix26]

That looks like fun!  However, you really need to read JD Mather's document that I referred you to earlier.  All sketches need to be fully constrained and dimensioned, and you don't need to model everything on your disk three times-- there's a polar pattern tool for that purpose.

Take another shot at the disk, being careful to constrain to the origin in such a way that you can make good use of origin planes and axes for symmetry.  Then post it here and we'll be happy to give you more pointers.

[JohnnyKash]

I've read over that, and done the constraint and dimensioning tutorials, but I don't really get them. I can't figure out how to fully constrain and dimension sketches; I don't know what I'm missing, or if I'm truly doing it right. And I don't fully understand what they're for in the first place.

This is my attempt at constraining and dimensioning a starter sketch for one of the wrist plates.

[JohnnyKash]

Okay, now I understand what constraints are for. I didn't see the Introduction to constraints until last night, didn't notice it in the tutorials list. Doing the hands-on tutorials without the primer wasn't a good move.

The last file I attached says I need two more dimensions. Those I still don't get. I've placed some already, but I can't find how to place the other two without overconstraining the sketch. What else does it need from me?

[JDMather]

I see you are using 2008 - see this page instead

http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

You need to Project Geometry (Inventor should do this for you if set up correctly as indicated in paper) and add a coincident constraint between the projected origin and the center of the circle (Inventor should do this for you if set up correctly).

You have dimensioned the size of the circle in a strange way that is not manufacturable or inspectable.

This is how I would dimension (not the Symmetry constraint added between the angled lines and the horizontal line).

[JohnnyKash]

For modeling the middle links that have the beveled faces, is there a more elegant solution than I'm thinking of using: extruding  "Cut" retangular prisms on properly angled sketch planes to remove material.

[JDMather]

Model it up best you an and then attach the attempt here.

Someone will then show you a better way.

[JohnnyKash]

I haven't gotten to modeling the beveled link yet, but I've been trying to get to it today.

I've drawn lines that should pass through the centers of the revolute joints in the middle link, once its modeled. I'm stuck for the moment because I can't draw lines of a precise length at a precise angle from an arbitrary point to another arbitrary point--how do I do that? Just using the mouse on sketch planes the numbers hop up or down with decimal place hangers-on. I need lines 150 mm long (my guess as to the length of the L-shaped links), each starting at the center-points of the purple circles that are parallel to the revolute joints in either wrist plate.

As you can see, right now I'm modeling it all in one part file to get everything to fit together just right* before I save each piece to its own file.

*If this thing isn't modeled perfectly, the mechanism is over-constrained and won't work.

I need to finish this this weekend.

[JDMather]

Workplane2 appears to be a dulication of the YZ Plane?

Sketch3 has duplicated dimensions AND duplicated Reference dimensions of dimensions.

With better use of geometry that sketch only requires 1 dimension.  (use equal (=) constraint and midpoint snaps)

Shouldn't this be multiple parts?  In Extrusion2 set the Option for New Body if it is a different solid body than Extrusion1.

I see no real purpose of Extrusion3 (make Extrusion2 to correct size to begin with.

Same with Extrusion4 and 5. Make one extrusion solid body and pattern.

Sketch4 - duplicated dimensions.

Extrusions 6-13 are duplications of work, duplications of earlier extrusions.  Use Patterned Features. In fact, because this will be an assembly of identical components - only need one.

I don't see the purpose of Extrusion15 - make Extrusion 1 correct to begin with.  You can always edit sketches and feature sizes rather than add addtional features.

Workplane8-Extrusion42 appear to be more duplicated work.  Get lazy!  Don't do duplicated work.  Mirror, or copy or pattern.  Same part in assembly.

Holes, more duplication.  Use patterns, or better yet, Component Pattern in assembly.

You control the length of lines by dimensioning from datums - just like person out on the shop floor who will manufacture the actual parts. 

I think this might be a bit too complex of a project for a beginner.

I recommend you purchase a book to go through.

I recommend you go through the Help>Learning Tools>Tutorials and Skillbuilders.

There are many other basic tutorials available on the web including - http://inventortrenches.blogspot.com/p/inventor-tutorials.html and the ones in my signature.

Reverse engineer every file posted here for the past 3 years and read the comments.

Learn how to use multi-body solids and assembly creation from the basic tutorials and then come back to this project.

You are working too hard.  Learn to make the software do the work.

[JDMather]

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@JohnnyKash wrote:

As you can see, right now I'm modeling it all in one part file to get everything to fit together just right* before I save each piece to its own file.

I need to finish this this weekend.

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You can still model in one part file - but as multi-body solids to get everything to fit together just right, but use multi-body and patterns to reduce your work.

You will not be able to finish this this weekend becuase it doesn't appear you have and any training and you are doing too much work.  Inventor is a professional program and deserves (requires?) a professional level of preparation.  I suggest that you go to your professor and recommend that your school add a class in Inventor taught by a certified professional.

[JDMather]

I noticed that it was 6 days between posting v1 and v3 of your project.

It should take about 20 minutes to recreate v3 correctly.

I just noticed that you are using v2008.

I was going to use 20 minutes to remodel - but you would not be able to open my file.

Multi-body solids did not exist in that version, but it would be easy to model this as an assembly.

Students can download Inventor 2013 for free from http://www.autodesk.com/edcommunity

[JohnnyKash]

I . . . I have to have it finished this weekend, or at least no later than Tuesday. I've got to get it made so I can import it over into Maya to attach it to the art project I'm working on that is due Oct. 8th.

I know I'm going about this inelegantly, some of the flaws present in the file I was going to remove--they're relics from me experimenting, trying to find the correct dimensions. It's not easy getting the proper relative dimensions from the image in the patent--that's why it took so many hours. It would have been quick work if they would have supplied an elevation view of the mechanism, without the perspective distortion on the dimensions.

I tried using the polar clone tool, but I couldn't find what to key it off of.

I will learn the right way, because I really like this program and plan to use it a lot in the future, but right now there's simply no time. What can I do?

I know the dimensions of all the parts now, I just need to be able to key lengths off of those revolute joints to make them to those precise dimensions. How do I dimension off of the dot in the center of the circle that is parallel to the revolute joint? Or do I add a workpoint there to do so?

I'll download the newest version this coming week. I can't from home because it would take a couple of days; my internet access is awful.

[JDMather]

To give you an idea how much extra work you are doing - all the geometry you created could be made from a simple sketch of 4 Rectangles (and a couple of construction lines) and 7 total dimensions.

See my sketch

[JDMather]

Here is an image of the solids made from my simple 4 Rectangles.

Note the Thickens were to add a bit of cut clearence to the holes so that the pins could rotate (an assumption).

(ignore the red line in the image - it has no significance, I must have moused over it causing it to highlight on my way to grabbing the screen capture)

[JDMather]

If I simplify it even more and make the geometry exactly the same as yours as single disjointed solid rather than multi-body solids the feature tree is far far simpler than yours.

[JDMather]

Here is breakdown of exact creation of your geometry (not how I would do it).

Revolution1 - Revolve the base diameter rectangle to create cylindrical base (a revolved rectangle results in a cylinder).

Extrusion1 - Extrude the two rectangles to make the "box" features - no need to extrude and extrude and extrude again to cut.

Revolution2 - Revolve the pin rectangle to creae cylindrical pin - you created Holes and then completely filled them in.  Why?

Circular Pattern1 - make pattern of Rev1, Ext1 and Rev2 - you recreated these features all over again, including the Holes that you then filled in.  (no clearance between the "pins" and the holes - therefore there was no purpose to making holes)

Mirror1 - self explanitory.  Why recreate that which has already been created.

Solving the problem of how to dimension a simple angled line requires a similar understanding (hint: Project Geometry) of how Inventor works.  Where is your instructor?

[JDMather]

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@JohnnyKash wrote:

 How do I dimension off of the dot in the center of the circle that is parallel to the revolute joint? 

I'll download the newest version this coming week. I can't from home because it would take a couple of days; my internet access is awful.

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See hint in previous post.

Attach your next attempt here.

[JDMather]

Just to emphasize how much extra work you are doing - here is side-by-side comparison of feature trees to get exactly the same geometry.

Spend a few minutes sketching (with pencil and paper) a plan for getting your desired geometry before starting in Inventor.

Once you get more experience - recognizing the underlying geometry (2d sketches/solid primitives) should become second nature.  This is how you get your work done in 20 minutes.