I am having trouble trying to get the Loft-1 to run the same shape as Revolution-2 .Picture 1-1 shows how Loft-1 is slightly off centre to Revolution-2 at the top .Ideally could i model the Loft-1 and Revolution-2 using different tools in one command making it a smooth shape. Another problem i have is how do i make Revolution-2 at the end terminate into Revolution-1 smoothly.I tried using Loft but it kept getting fail message.Picture 1-2 shows where to terminate the end into the Revolution-1 body.
Is there a more correct method to create this shape then what i used.Any suggestions you could recommend and i will attempt.
Any help appreciated
I don't have the educational version of Inventor to hand, so unfortunately I cannot post a model that you can open here, but I have taken a look at the model and can see the issues you have described. I don't think there is any major issue with your current choice of modelling tools, but I think a key to helping you making the shape you desire is to create multiple solid bodies, and then Combine them at the end.
When you create Revolution2, choose to make it a 'New Solid' rather than 'Join'ing it to Revolution1. Then, when you create Loft1, select the free circular face of Revolution2 as a profile (rather than Sketch3), and you will be able to define tangency between the Loft and this Revolution. (If you want this transition to be smooth, I would also recommend making sure the centreline for this Loft section (Sketch4) is tangent with the Revolution.)
As for the apparent 'misalignment' of this Loft (1-1.png) - I think the shape is as expected given the reduction in diameter in this Loft, and intersection profile between this and the main body (as multiple bodies, you can make Revolution1 invisible to see how the Loft actually flows). Moving Sketch5 outwardly might give you the shape flow you were expecting, but this means the circular sections are no longer in line. Alternatively, you could use a Rail Loft or Area Loft here instead of Centreline Loft to offer you more cross-sectional shape control. But I don't think there is anything unexpected happening with the shape as it is.
To make the pipe 'blend' into the main body (1-2.png), I think you were correct to try using a similar Loft here too (after building a new circular sketch where you want this to 'enter' the main body). Perhaps you will have better success here when using the multi-body approach. If the Loft is still unexpectedly failing for you, you can post the input model here and I can take a look at what's going wrong.
After completing the entire pipe shape, use the Combine tool to make these into a single solid, allowing you to Shell & Fillet the whole model as previously.
As for using a single command to create the entire pipe shape: you may be able to achieve what you want using a single Sweep or Centreline Loft command, but both of these have limitations compared with your current workflow (Sweep only accepts one profile shape, so reducing the pipe diameter at the exit requires you to create a complex guide curve; and Centreline Loft might not give you the same precise torus shape as a Revolution/Sweep will in the constant-section region of the pipe). You can experiment with these options and see if these give you a better result, but as I say, I don't think your current workflow has any inherent problems.
Incidentally, the excellent 'The Creative Inventor' magazine featured a full tutorial for modelling a volute part earlier this year (Jan/Feb 2011 issue); I would recommend taking a look at this as the tips here may be useful for your model too:
I hope this helps you to continue with your model, but please feel free to post again if you have any further questions.
OK i used some of Jakes recommendations and this helped.I have a small dent (picture attached) .How can i modify the Loft-1 to Revolution-2 so to have this section all blend in together without the dent ? Do you see any problems with this shape or can it be better modelled?
I will tidy it up and fully constrain all the sketches when i redo.
Actually Jake just got married and is on his honeymoon "vacation", something he failed to add in his reply.
.... no access to Inventor (or even a PC ).
Jake - no computer?
Your giving her an unrealistic view of the future.
Hi! I took a look at this case and I think I might have come up with a reasonable solution here. Please take a look at the attached part. This is not a simple body to model in any 3D Solid CAD package, including Inventor. Here are what I found from the exercise.
1. It is unrealistic to expect the geometry to be created purely by 3D solid features. 3D solid features are convenient to construct realistic model. However, it does have a limitation in terms of managing interesection and timming unwanted porting. The model has to be done via surface modeling and then turning it to a solid.
2. The key to success here is how you manage or regulate the intersection. Based on the design requirement, the tapered inlet has a conflicting design constraint to the pump body: the inlet has to be round and tapered and it has to intersect right at the cylindrical edge of the pump body having a big sphere side face. I am not aware of a solid modeling technique accommodating this type of conflicting constraint.
3. Inventor is a feature-based parametric CAD. Each piece of geometry has to keep full associativity to its parents. A curve cannot arbitrarily be created out of nowhere or a face cannot be trimmed as one wishes without a toolbody. Everything you create has to have a source or a reference. This behavior can be perceived as inconvenience in some cases.
Let me know if you have any question.
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