Impeller Headache

[DaleLloyd7569]

Hi

I am fairly new to Inventor but have managed to figure out most problems I have run into myself. However I now need to model the impeller on the left of the attached PDF drawing and other than the main boss I really don't know where to start as it isn't a straight forward blade design. Any help on this would be greatly appreciated.

Thanks

Dale

[JD Mather]

Ahh, I see the problem - your drawing is upside down! :lol:

OK, now that I've had a good laugh can you zip and attach the ipt with what you have been able to do so far?

[Rob123]

Ive added a quick 2 min drawing , its rlly nog that hard to make, but i hope you know how to use work plains :unsure:

[Rob123]

just ^^ try to draw it the same way i did :)

[shift1313]

that should be a fun one:)


it looks like you have some fairly planar cross sections to work with so thats nice. I would draw the 3 cross sections givent at their location in the plan view. Looking at your elevation view the lower edge of the impeller appears to be planar so i would create a plane, draw the top view and project it down onto that plane. You also have a nice reference in the elevation view for the cross section of the top of the blade. I would use all these in a loft operation.

Id have to sit down and give it a shot later(cant right now) to see how this would all work out.

[JD Mather]

...a quick 2 min drawing , its rlly nog that hard to make...

"rlly nog"? Looks like 2 minutes of work.



...just ^^ try to draw it the same way i did

I prefer a more robust approach - but I'm rather slow at 5 hrs effort.

[DaleLloyd7569]

Sorry I didn't send you what I had done straight away but I have been trying the method suggested by shift1313, but with not much success. I can see by your image that it can be done but I have to ask... how?...is it done using the sections and a sweep because it wont work for me. I have attached what I have done so far

[JD Mather]

Read these threads, this is a difficult part, before you can continue you must learn to constrain sketches.

http://www.cadtutor.net/forum/showthread.php?t=34878

http://www.cadtutor.net/forum/showthread.php?t=33399

http://www.cadtutor.net/forum/showthread.php?t=33317

[JD Mather]

Create a sketch on the XZ Plane as shown and then attach the file here and I can walk you step-by-step through a solution to the problem.

[JD Mather]

I also noticed you are on SP0. You should install Service Pack 1. I have a nice solution to your problem when you are ready to continue.

[DaleLloyd7569]

OK I have read the other articles and have worked through your MA105-1L tutorial, I didn't realise it was so important to have everything constrained. I have restarted the impeller part but I haven't gone to far with it as I am not sure if I am going in the right direction. According to Inventor the whole sketch is fully constrained but there does seem to be a lot of dimensions. I have attached the restarted part, am I on track so far? On a separate note I think the derived part tool which was in your tutorial will be useful for me when I want to make the pattern plates.

[DaleLloyd7569]

Just noticed your other post, just shows you should check all the replies and not just the one you get an email for.

OK I have done the sketch as per your post, is it necessary to fully constrain a sketch because it still says it requires two dimensions which when I put them in don't seem necessary.

Ignore the attachment to my previous post the correct one is here

[JD Mather]

I have a realy nice solution for you on this problem if you stick with me.

In the last file you attached the Sketch1 turned color indicating that it is fully constrained.

There are two Extrude features that should not be there. Delete those two Extrude feathures.

The next step is to create a Workplane offset -160 from the XY Plane. (see steps 1-3 in attached)

Then start a new sketch on the offset workplane and Project Geometry the line indicated in step 4 in attached image. Let me know when you have completed these steps.

[DaleLloyd7569]

OK I have done those steps

[JD Mather]

Now,
Create a WorkAxis through the center of the R387 arc.
You can do this by selecting WorkAxis and then clicking on the endpoint of the construction line and the perpendicular sketch plane (I believe your sketch was on the XY Plane).

[JD Mather]

Next create a Coil surface.

The command will try to select your closed profile Sketch1 -
Change the Output to Surface see 1
Now you can select the projected line created in Sketch2

Your coil won't look like the attached preview yet - don't hit OK just yet.

[JD Mather]

While in the Coil dialog box click the Coil Size tab and set as shown below.

[JD Mather]

Click OK and you should have a yellow or orange translucent surface.

Select Extend surface and then click the three edges to extend as shown below. Set the extend distance to 10.

Let me know when you have completed this step.
Believe it or not - you are almost done.

[DaleLloyd7569]

OK All done

[JD Mather]

Now Extrude - To the surface.

Then right click on the surface in the browser and turn off the Visibility of the surface.

[JD Mather]

Then add a Varialbe Radius Fillet along the edge shown. Your Start and End radius might be reversed depending on where you pick the arc - doesn't matter as long as you have the visually have the 125 and 70 on correct ends.

I forgot to arrow the important entries in the attached image so study it carefully to see that I am on the Variable tab of the Fillet dialog box.

You might be wondering by now where I am coming up with some of my dimensions. I'll explain that in a bit - and if you want to change any dimensions that is easy enough to do as it is a fully parametric model.

[JD Mather]

Now as the R38 Fillet to the outer edge as shown.

[JD Mather]

Select the Shell feature and then click the 3 faces shown. Set the Thickness to 16mm and click OK. Let me know when you have completed these steps. One more tricky step and the rest is gravy.

I realized that I might have confused by having the three arrows going from the selection tool it will be active when you start the command - you do not need to click that icon - just click the 3 faces as shown.

[DaleLloyd7569]

OK all done, but you are right i can't see where you got your radius dimensions from

[JD Mather]

OK all done, but you are right i can't see where you got your radius dimensions from

I'll get back to that and suggestions on how to edit once we see all of the geometry.

Create the sketch as shown on one of the origin workplanes (I'll let you figure out which one to make it look like attached.) I assume by this point that you are starting to anticipate my method. On your drawing it shows the 5 dimension as 3, but do it as 5 for now. Notice the position of the Origin Center Point. Everything I do is in relation to the origin.

Once you get this sketch Revolve the feature.

[JD Mather]

Add R8 fillet to edge shown.

[JD Mather]

The order in which you place fillets is critically important.
Add the Variable radius fillet to the inside edge as shown.

[JD Mather]

...add fillet to bottom inside edge as shown.

[JD Mather]

...add the fillet to the upper outside edge.

[JD Mather]

and last fillets

[JD Mather]

Select Circular Pattern and be sure to click Pattern Entire Solid as shown with the red arrow in attached image, then select appropriate origin axis in the browser.

[JD Mather]

I started out with parallel sections exactly like the original drawing.

As I started constraining it became obvious to me that the original designer fudged some dimensions as they didn't have the advantage of a parametric geometry solver when working on a drawing board.

I decided that even on the drawing board radial sections would have made more sense than parallel sections. I could argue the parallel sections aren't even drawn correctly - the round ends would be ovals in a true projection. See my image of the same sections imposed over my final solution.

To get the final solution I adjusted the variable fillet dimensions to fit the given section dimensions as closely as I could. If these dimensions don't suit you simply keep adjusting till you get what you want.

If my entire technique doesn't solve your problem, all I can say is good luck!

I think you can figure out the hole.

I hope I was of some help, even if this solution doesn't solve your design problem.

[DaleLloyd7569]

Thanks very much for all your help. I came to the same conclusion on the dimensions when I first started to draw it. The impeller blade can't be drawn using all the dimensions shown which actually means the sections don't quite line up either. I think the client will be happy with this model and I have sent a copy to him to evaluate and explained about the dimensions on the original drawing. I have managed to figure out the hole myself, and also the circular pattern.
Once again thanks for your time and effort, I have learned a lot over the past few days but I also realise there is so much more to learn!

[shift1313]

wow that is some step through JD!! i want to draw it now:)

[JD Mather]

i want to draw it now:)

To really appreciate the end result you should try without looking at my solution (OK, too late for that). I did 4 iterations with the first 2 much more complicated than the final solution. I find it a fun challenge devise really simple and robust solutions to what seem initially to be very complex problems.

[shift1313]

all i did was look at all the pictures :-D

[pgcust]

once again J D shows us why we use inventor,as a self taught inventor user i appreciate all input from all forums,but J D's tutorials keep me wanting to keep trying to improve my skills
thanks J D

[Lazer]

Great tutorial JD:)