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. 

[JDMather]

Create a circular pattern of the entire Solid as shown, select the appropriate axis from the Origin folder in the browser. 3 copies (see attached image.

[JDMather]

Expand the Extruded feature in the browser and right click on the sketch and select Edit Sketch.

Add the center point rectangle clicking the two points as shown in attached image.

[JDMather]

Add the two dimensions as shown and then exit the sketch.

Right click on the sketch in the browser and select Visibility.

[JDMather]

I forgot a step - but we can do it now.

Add the Fillets as shown. (in attached image)

[JDMather]

OK, now we can extrude-cut the new rectangle we just added.

Cut through all mid-plane.

[JDMather]

Start a new sketch on the plane perpendicular to the first sketch.

Project Geometry the apex point of the triangle.

Create 10mm circle centered at the projected point.

Extrude-cut mid plane (symmetrical) through all.

Circular Pattern the last two Extrude Cut features that we made. 3 copies around appropriate axis.

Attach your progress here.

[Anonymous]

Thanks a lot for this. The first thing I did when I woke up was starting this, and I've now spent less than an hour and I'm nearly where you left off. This is absolutely amazing. I've already learned more from you than I've learned on school the few weeks we've had this. 

I've attached two files, one .ipt that shows my progress and one picture that shows my lack of knowledge on this. On the picture, I've tried to use the Circular Pattern to do the last two Extrude Cut features. When I click ok on the picture, the one that you/we have extruded already, is made 'solid' again like the other two branches. 

I've tried and went back and forth a bit, but I'm not sure what I'm doing wrong. I'll mess around with it, and if I figure it out I'll post here asap.

Your help has been fantastic, and I'm so grateful for this. Beyond belief. 

Edit: I think I figured out how to to the Circular Pattern to do the Extrude Cut features. Replaced the old file with the new one.

Edit 2: Therefore you can just avoid the picture attachment. 

[CCarreiras]

Hi!

Maybe JD is now taking a nap in the states... I will help... from europe until he come back  (This became in a international Project!!!)
Let me see if you evolved your acknowledgment about inventor !!!

The question of your circular pattern is ... you are choosing the ALL SOLID to pattern, and this is wrong for this case because you only want to pattern some FEATURES, right?.

You have to create this pattern using the first option... "Pattern Individual Features"... then:

Then  click in "rotation axis" and select the axis from the origin folder in the browser... if you design the part centered, you may use one of these axis to do the rotation ... then is only input the values, like you had before in your first attempt.

Try it...

[Anonymous]

Yes, I figured that out later, as you can see in my attached .ipt file. I'm sorry if my edits wasn't clear enough.

And thanks for stepping in! I really think I can learn how to do this with your help, and I've already learned new techniques to help me speed things up, that we haven't even look on at school.

[JDMather]

Back from my little nap..... 

I see you figured out the difference between Solid pattern and Feature pattern.

Start a new sketch on the face of the part.

Hit H on the keyboard and click on the point in the center of the face.

Enter your hole information. (select Threaded hole type)

Next part!

[CCarreiras]

He's Back!!!

GG, you'll be in good hands, excellent teacher, take the opportunity to learn.

Bye... good work

[Anonymous]

Having some issues with my computer, and I have to rebot. I'll be back asap, finishing up part 6 (or part 1, I'm confusing myself here, will have to check the pictures once my computer is back on) and attempting part 5 as that's the scariest part right now.

Thanks for continuing on this. You really are an amazing teacher.

[Anonymous]

The part we've done now must be part 1. I've attached the file I consider as 'done'. Now I'll open a new file and attempt part 5. I'll try to implement the techniques I've learned from you, but I suspect it might be too soon to have controll of that now. But I'll give it a good go and attach the file here when I feel I've done as much as I master right now.

Edit: I've now fooled around with part 5 a little, and I've discovered that my initial plan has failed. I wanted to make the the top of the screw, then add another sketch on the face of that one, and add 6mm fillets to get the right dimention. Sadly, I can only add fillet on the bottom of the screw, and that really isn't helpful at all. 

Any suggestions here? Am I onto something here, or am I just as far off as I was with part 1?

[CCarreiras]

Hi!

You can do that in 3 operations:

1. Revolve for the body
2. extrusion for the hole
3. Thread.

Start to sketch alf of the body. Make a centerline connected with center point, Fully constrain that sketch with constrains and dimensions.

[Anonymous]

Ok, I understand.

As I'm not familiar with this kind of drawing, should I sketch the whole body in half, then revolve it, then add fillets, holes and thread? Or should I sketch it in 4 parts? Screw head, threaded part, the sphere and the part inbetween the sphere and the threaded part?

It's a bit confusing to me, but I'll do my best to understand your instructions. 

Thanks a lot.

[CCarreiras]

Do it like you told first.

"As I'm not familiar with this kind of drawing, should I sketch the whole body in half, then revolve it, then add fillets, holes and thread."

Try your best and when you stop, post the ipt.

[JDMather]

---

@carloscarreiras8703 wrote:

Do it like you told first.

...sketch the whole body in half, then revolve it, then add fillets, holes and thread."

Try your best and when you stop, post the ipt.

---

Follow Carlos instructions.

Attach your file whenever stuck.

[Anonymous]

I'm getting started at least, I'll continue on this ASAP, but I have to run some errands first. I'll get back to this ASAP as I said, couple of hours at most, I hope in an hour tho.

[Anonymous]

I attempted to draw half of it, but I can't figure out how to do the sphere on the end.

Also, I feel I'm doing something wrong in terms of the diameter of the threaded part since it looks like it should be fillet later on, and then it'll be too small. Any inputs here?

Thanks a lot again guys. I feel like I should go on and on with thanking you guys, and I really should to show my true appreciation, but unfortunately I wouldn't have the time to do that heh. Hopefully you understand how thankful and grateful I am that you're taking the time to help me out on this. Appreciated beyond belief.

[Anonymous]

Your appreciation is shown with the dedication you are putting forth.  Guys like JD enjoy helping others as long as they show that they are willing to learn and are most importantly putting in the effort.  Just continue to ask questions, post your attempts and keep an open mind.  You can always tell the difference between people that just want someone to do the work vs the people that legitamately want help and are gaining knowledge/ experience.  Kudos to you and the helpers!