Help needed for advanced homework.

[Anonymous]

Hi.

I just got this paper handed out that's due this friday. I like to start early on these things, and although I feel like I don't have too much time for this particular assignment, I couldn't have started any sooner.

I'm not looking for someone to do this assigment for me, I'm just looking for some helpful tips, and a walkthrough would be perfect but I doubt anyone has got the time for that. 

The problem for me is that I haven't used inventor before. We started using it on school two weeks ago and I've done all the exercises, but this seems beyond me. Any help as to where I should start, how I should do it etc would be immencely appreciated.

Right now I've done part 6 just to get started, and I'm starting on part 6. I'm unsure as to where to begin..

Any help and discussion appreciated!

Edit: I'm using Autodesk Inventor 2013 professional.

Edit 2: If there's a problem with the language, I'll be happy to translate whatever you need to understand it instantly. I just figured the images and measurements should be enough, but I clearly understand if anyone has any questions about the other text. I'll obviously answer any other questions as well related to this.

Edit 3: Any feedback is appreciated. If there's something wrong about this post, the info I'm giving etc. 

[Anonymous]

For the bottom Sphere....

Draw a 3 point Arc.

1.Start at the end point of your sketch

2, Drag your mouse along the centerline to the desired diameter of your sphere (in your case it is 11mm)

3.Drag your mouse perpendicular to the CL until the Tangent Constraint appears.

This should generate a half circle that is 11 mm in diameter.  Once completed, Finish Sketch and revolve around CL.

As for Fillets and Chamfers, I typically do those features after once the main shape/ body is complete.  Others do the fillets or radii in the sketch and that is fine too.  I suppose it is a preference or how you were taught.

[JDMather]

Note the differences between my sketch and your sketch.

Do not make up dimensions - use the manufacturing inspection dimensions (drawing dimensions) if possible.

You can ignore the two full circles for now (Ø1.3 and Ø12).

You can get diametral dimensions rather than radial dimensions by clicking on the centerline rather than on the end of the centerline.

[CCarreiras]

Hi!

Draw the red geometry. and trim what's in excess. Are you familiar with the tool "Trim"?

and thats it!!! Revolve!!!

[JDMather]

Here is a close-up detail.

I used the Sketch - Split tool to split the arc into two pieces and change part of it to Construction.

I don't think this is required to get the Revolve profile, but that is what I did.

[Anonymous]

Alright. I've 'made up' a few dimentions that I didn't know how to implement otherwise. Such as where you have '4' where the threaded part starts - I had no idea how to do that other than calculate the dimentions using your sketch.

I was actually quite happy with my progress this far since I felt I had figured out a lot, but I guess I'll have to go back to my sketch now and edit those 'made up' dimentions?

I'll attach my current progress.

[JDMather]

I put in the R4 fillet in the sketch.

As noted - fillets are usually put in as features (as you did it).

You have two threaded features in your history tree.

And not the i in circle.

The shaft is actually the wrong size Ø24.5 for the thread.

I think I would make the change and point out the error on the drawing to the instructor.

(there were also a couple of other error/missing dimenions on some of the other parts, but these were more minor)

You have the spherical feature in the wrong location (tangent to the end of the shaft) - this obviously can't work).

[Anonymous]

I've tried a little more now.

I can't figure out how to make the hole in the top of the screw. I've added a point in the sketch, but the hole function won't put a simple hole here - why is that?

Also, I think I got the sphere right now. 

About the shaft and thread - I'm sorry but I don't understand what you mean. I've followed the instructions perfectly I think. The shaft should be Ø24,5, and the thread is the same type as stated in my assignment.

Two steps forward, one backwards I guess, but if you can deal with my incompetence I'll work hard towards finishing this. I'm already looking forward to the awesome feeling I will get when I've learned how to do this.

Thank you, once again, for your help.

Current progress attached.

[Anonymous]

The hole is a bit tricky. You need to make the sketch for the hole Tangent to the surface of where you want it placed.  For your example, you need to create a plane tangent to the head.  Once your plane is set, you will then do a sketch on that plane.  Then locate the hole with dimensions and constraints.  Finish Sketch and use the Hole Command.  Select the point and be sure Termination is 'Through All'. 
See my screen shot below..... Note that you do not need the point you added in your Sketch 1 (Revolution).  By removing this point, you will now notice that your sketch is Fully Constrained!  That my friend is a good thing!

Hint: Always have Origin Planes on and Project them in sketches when needed!

[JDMather]

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@Anonymous wrote:
 

I can't figure out how to make the hole in the top of the screw.

About the shaft and thread - I'm sorry but I don't understand what you mean. I've followed the instructions perfectly I think. The shaft should be Ø24,5, and the thread is the same type as stated in my assignment.

 

 

[Anonymous]

I don't understand everything you say here, but I managed to get the hole I wanted!

Does this part look ok now? If so, I'm ready to move onto part 3 and 4 (Tapp and skive), I think they go pretty much together. I really should've translated this before I made the post if I knew you guys were this helpful. Next time...

[Anonymous]

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@Anonymous wrote:

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@Anonymous wrote:
 

I can't figure out how to make the hole in the top of the screw.

About the shaft and thread - I'm sorry but I don't understand what you mean. I've followed the instructions perfectly I think. The shaft should be Ø24,5, and the thread is the same type as stated in my assignment.

 

 

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I'm not sure why you are quoting this, but I'm not trying to sound arrogant or anything. I honestly feel like I've followed the instructions as stated in the assignment, and I can't see how or where my modeling is wrong.

I do believe you though, I'm just not capable of seeing/finding it.

I'm a little anxious that I might run out of time for this project, but there's over 24 hours left, and I'll spend as much time as possible on this forum and on the assignment in general, so let's just see how far we can go.

And I can't stress enough how highly I appreciate the help every single one of you is giving me. If I at any time sound arrogant or even anything close to that, I'm sorry, but my behavious is clearly misunderstood then. I'm humble, open minded and seeking to learn from your knowledge.

[JDMather]

I just realized that I made a mistake too.

The designation of 24x5 means a diameter of 24 with a thread pitch of 5mm. (distance between threads, not thread height)  We use a cosmetic texture to represent the threads.

The diameter of the shaft should be Ø24 NOT 24.5.
I was not paying attention earlier and didn't go back and check the drawing - it is correct, our model is incorrect.

[Anonymous]

Alright, I've edited the dimention for the difference between the threaded part and the screw head to be 8mm (up from 7,75mm).

Does my part look done now, or do I have some errors still?

[Anonymous]

I will be heading off to bed for a few hours. Hopefully I can finish  this tomorrow, and I'll be as active as I possibly can on this forum and working on the drawings/modeling myself. 

First thing tomorrow is checking this thread for replies, and see if I'm done with part 5 or not, then I'll fix anything that's needed to be done with part 5 and move on to part 3 and 4 next.

This is undoubtably looking good so far. Regardless if I'll get this done in time or not, I've learned a lot and I'm really enjoying using this program.

Thanks again for all your help so far.

Edit: Also, I don't want to throw out a lot of unfinished sketches out here. I want to show that I'm dedicated to learn to model the parts one by one rather than throwing out everything just to get it done so I can hand in my assignment. That's not what this is about. I want to learn and enjoy working with Inventor, not just please my teacher, and I think the best way to do that is to fully understand how to model each part before moving on to the next one. And I have to admit, I'm really enjoying this so far.

[JDMather]

You still have 2 thread features on the part (see attached).

Delete one of them.

You should be able to finish the rest of the parts in 10-15 minutes each.

Then you will need to figure out how to assemble (tip - assemble 1 complete and then circular pattern).

[CCarreiras]

HI!

Very nice! youre getting better!!! and the part it's almost perfect...

But... you want to finish this part like a Boos??!!

See the PDF attached. follow it and you will have a cleaner part, with less steps.

If you dont understand something, ask.

Tip: It´s important to understand when use split or trim. Can you tell me why? This is my challenge for you 🙂

[Anonymous]

One again, huge thanks to both of you. And Carlos, I can't believe you took the time to do all of that, thanks a lot!

I would assume the split and/or trim functions are used to, in my case at least, make the sketch look cleaner and remove excess geometry. For instance, I didn't need to revolve cut a whole circle as I only needed half a circle (arc?) to get the job done.

I have attached the file once again, and I think I'm (we're!) done now. I have a lecture in an hour that lasts for an hour, so I'll be back asap to start on part 3 and 4 unless you have any input on what part I should do next.

Huge  thanks to both of you again. I wouldn't even be close to do this alone.

[CCarreiras]

Hi!

It's done!!! very well. like a boss 🙂

The question between using split or trim:

Somethimes Trim clean  beyond we need and thereby can delete some constrains. With split, the geometry doesnt stand so "clean", but on the other side, we mantain the struture. e.g, its easily to control de dimensions and position from a circle thean a arch. With experience, you will leran when its better use trim... or split.  You will use Trim often 🙂

Go on to other parts. you are close to get your degree in Inventor.

[Anonymous]

Thanks for clearing that up.

Now I've moved on to part 3, which looks incredibly simple, but of course I had to stumble accross a few problems here as well.

When I want to revolve my drawing around the centerline axis, the color of the pin turns brown instead of the usual silver color. Why is this, and does it matter?

My plan from the attached sketch is to revolve it, fillet and chamfer wherever needed, then attempt to extrude cut the hole. But first I obviously need to revolve it properly.

Any input on the sketch so far?

[Anonymous]

Your part turned "Brown" because it was making a surface instead of a solid.  I believe the answer lies within your sketch.  Your axis is both a Centerline AND a Construction Line.  Click on your axis and note that both options (Centerline and Construction) are activated.  You require the line to be JUST a Centerline.  Once you change this, you should be able to revolve your part as a Solid.

As for the sketch, it is Fully Constrained and the dimensions make sense, so you are doing well! Keep going my friend!