CAD Software Modeling boat tail - Inventor 2020

[opcon]

Greetings!

I'm trying to model the boat tail of the MAC Performance FireStickXL - 3" dia. rocket and I've hit a wall.

After researching and some trial and error (/cough manual searching in the 'data') in Excel I figured out how to calculate the Ogive radius thanks to this website but I'm still a bit off track. I'm working backwards from an OpenRocket file provided by MAC Performance to provide dimensions.

Likely, my maths are off, but I'm unable to spot where. Basically, the aft throat of the tail is off, it should measure 60mm in dia, but I'll be darned if I can get any closer than 58.569mm.

If anyone has time or inclination to let me know what I'm doing wrong, I suspect the Ogive radius (p) is not correct.

Attached spreadsheet, ork and ipt inside attached zip file.

-With love, Opcon


Attached rendering

 

[TurbulentSphere]

Ogive is just part of a circle, so I use arc segments in the sketch and constrain it to the dimensions I want. No math required.

 

[opcon]

Ogive is just part of a circle, so I use arc segments in the sketch and constrain it to the dimensions I want. No math required.

How do you go about obtaining the correct second arc coordinate?

 

[jbr]

really easy in fusion, just make a nosecone and chop it where you need it

 

[opcon]

Ogive is just part of a circle, so I use arc segments in the sketch and constrain it to the dimensions I want. No math required.

Ok, with your feedback I was able to progress quite a bit. Thanks folks.

 

[opcon]

I ran into another road block, and I thought I would share this learning experience with you. This may have been a trivial issue for experienced modelers, but I nearly threw in the towel here. Attaching fins as components or fin assemblies to a motor mount cylinder is more difficult than I thought it would be. I'm new to inventor but bear with me as I try to explain the problem and solution that I'm happy with.

I had finished modeling all the components, I built joints and put all the components together in an assembly and saved the fins for last. This was a mistake. I should have started with the motor tube and immediately attached the fins before progressing. Another mistake I made was not knowing about the Manage -> Make Component workflow but I'll try to stay on topic here.

The only joint I could make work to attach a fin to the motor mount tube was the rigid joint. It attaches the fin to the center line at either end of the tube or the mid point of the center line not sure if this is normal or if because my motor tube extrusion was created with symmetry across the x axis of the x,y plane. Again, I am learning by trial and error here, I should probably get an Inventor book to learn how to use this software correctly.

I could not constrain this joint to mate the fin to the OD surface of the motor tube. I tried many options, researching the Interwebs and YouTube and found that some helper geometry in the fin component was the only option I could make work. I'll mention Manage -> Make Component here again because keeping UCS between components is a lovely thing.

My solution was to add a new solid body extrusion (in green) to the root edge of the fin tab in height equal to the OD radius of the motor tube, basically increasing the fin tab height.



This pushed the fin out from the center line and makes the illusion the fin is attached to the surface of the motor tube OD, however the helper geometry passes through the center of the motor tube, not a deal breaker.



Going back to the fin component, I toggled the visibility of the solid body helper geometry and in the assembly I now have a fin correctly sitting on the OD of the motor tube and have not broken any relationships in the process that make fine tuning adjustments in the future impossible.



I've had to walk away and come back at this many times over the past couple of days and it was really starting to bum me out that I couldn't get it to work. Lessons learned, view time as not your enemy but as your friend and don't try to make it work, make it work. I choose to model this rocket because I knew it would challenge my abilities and it has lived up to that expectation. Sure you could model this as a fin can using simple extrusions, but it would not really be modular and you break the iterative design qualities of using Inventor.

I'll post a final render when I'm done.

 

[opcon]

What do you think?

 

[dr wogz]

Opcon,

Learn about work planes, they are powerful features to work with. Also know about work axis, as they are also a big help with 'round' things..

You should have 3 constraints:
1. mate/tangent, for the fin to BT,
2. face to face, for fin placement left or right of the tube,
3. finally, face to face (offset) to align the fin up & down of the tube.

once the fin is properly constrained, you should then be able to do a polar array, so you do't need to constrain the same fin 3 more times. You should have a work axis thru the axis of the BT.. drawing on the intersection of two work planes / at the center of the cylinder. Cylinders & round things should always be drawing with the center on the intersection of two work planes for easier assembly down the road.

Your first constraint should be the face of the fin and outer the face of the tube, to get a tangent constraint. You could, if you wanted, also do a face to face constraint with an off set of 1/2 the tube dia. That is, the face of the fin and the work-plane of the tube (assuming you've made the tube as stated above. you could also have a 4th work-plane, parallel to teh X or Y work plane and tangent to tube.. but that's gettign sloppy..)

Second, your fin should have a work-plane thru its center. This allows you to constrain the work plane of the fin thru the work-plane of the tube. Your tube should have a work-plane (two preferred) on the X and Y planes, this should intersect at the center (center axis) of the tube. This will constrain it left & right of the tube

You then need just add a constant between the end of the tube (tube end face) and the fin end face. Again, either pick the flat faces, or pic a face & a work plane.. This constraint controls how far up or down the tube the fins sits at..

Knowing work-planes, you can easily manipulate some really odd-ball shapes!

 

[opcon]

Thank you for the feedback. I gave this a shot this morning and wow, that's a whole lot easier than the craziness I did to make it work. I didn't even realize you could constrain planes together so much easier and your instructions were very easy to follow. Thanks again.

 

[dr wogz]

30+ years with CAD & parametric modelers! I've picked up a few things!

glad to have helped!

Seriously though, work planes, work axis, and work points can make your modelling a whole lot easier! and you can turn them on & off (hide) as needed.

you can also constrain edges, vertexes, and a few other bits of geometry. If you wanted a strut or some other 'thing' connected to two fins, at a 45° angle, you would constaint the edge to face, and edge to face on the other fin, then a face to face angle offset (45°!) and finally a face to face to move it up & down.. That should give you a 'thing' connected to two fins, regardless of what measurements you have..

 

[opcon]

Paul, work planes and work axis are amazing for modeling rocket parts and assemblies. It's so much easier and far less complicated to make constraints that don't require offsets or crazy helper geometry, just let the work plane/axis do that for you. Thanks again for the help.

 

[dr wogz]

you can have work planes based off other work planes!

If your parts are designed right, you can have your assemblies rely almost solely on work planes, points & axis..