CAD Software Give me stuff to CAD.

[cwbullet]

I am willing to work with you on some projects,

 

[NTP2]

Aerotech Cases

There are some out already, but if you want to ease yourself into CAD, a good set of models for the Aerotech Cases / ends, plus a good set for the single use too. Some of the case cad models floating around are pretty bad. There are good ones too. but nice to have a clean set that has been verified including the tolerances. End up with a set of IGES / STEP files. STL maybe.

You can keep it simple (just cylinders) or add all the threads, chamfers, knurling, bevels etc. Dimensions are all on line. Modeled to the MMC (Max Material Condition) of the tolerance.

Mike K

Bonus points for .3DM files

I don’t see all the dimensions needed on the assembly drawings it looks like I’d need to get my dad’s calibers and measure the only case I have the 29- 40-120. I could do a cylinder that fills the space as a motor but you don’t need CAD for that…

 

[NTP2]

I am willing to work with you on some projects,

Wow thanks! What do you have in mind?

 

[Sandy H.]

I've been on Inventor since 2005. While it has quirks compared to other 3D Parametric packages, they also have quirks, so learn to use the tool you have as effectively as possible, IMO.

I have done large machine design (1000+ major components and tons of drop in parts like fasteners etc.) and learned over the years that the best thing to do is to take a breath before modelling a part. Think about the XYZ orientation of the part in its final position before starting the sketch. Decide if it makes sense for the XYZ origin to be at the left edge of a round pin or if it makes sense for the origin to be at the centerline of the pin. It makes constraints easier when doing assemblies and only takes a minute of thought to start at the right spot. Much harder to change later in the design.

In my opinion, always do this thought exercise, even if you're just sketching a part. Assume it will be used in an assembly and think about the end use of the part. For a nosecone, for example, you could build up the model from the bottom of the shoulder up. Or you cold make your XYZ origin the top of the shoulder and bottom of the nosecone shape. If done the second way, you'd constrain the XYZ origin to the top of the bodytube vs. doing an offset if it was the bottom of the shoulder. True, you could do constraints based on the features, but if you can constrain to the origin, it can be helpful as you iterate design. None of this matters for doing a 3D print, but if building an assembly in CAD, it can help a bunch.

Good luck with your projects. CAD (2D or 3D parametric) are just tools to let your creativity be realized. Focus on being good with your tools, but the real task is to be creative and invent, not just to draw and draft, IMO.

Sandy.

 

[NTP2]

Good luck with your projects. CAD (2D or 3D parametric) are just tools to let your creativity be realized. Focus on being good with your tools, but the real task is to be creative and invent, not just to draw and draft, IMO.

Sandy.

I look at it like painting, you start by copying the great paintings and get good with the tools and techniques of painting at the same time you’re developing your style and applying it to the copy’s, modifying here and there and before you know it you are doing completely original paintings.

 

[NTP2]

I don't suppose anyone knows how to do an ogive curve? google was not helpful.

 

[Bravo52]

I don't suppose anyone knows how to do an ogive curve? google was not helpful.

Ogives are just plotted curves. The math part is figuring out the boundaries and frequencies...about a thousand of them to get a smooth line. There are programs that will do it for you and I think even MS excel will do the math for you. Google "Nose Cone Design".

 

[Rschub]

An ogive or as we use it for rocket nose cones a tangent ogive is just a circle segment in cross section.

In Solidworks I use the revolve command and draw a half cross section of the outline as shown below.


The R66.43 is the ogive part of the sketch. The important part is that the center point of the circle is located on the vertical hatched center line. This makes the circle tangent to the body tube. For a ogive that is not tangent you can locate the center point of the circle anywhere needed. I put a little .25 radius on the nose to make it more accurate to the actual part but this is not necessary. This particular nosecone is a model of the LOC 7.5 nosecone.
LOC gives dimensions for a lot of their parts, making it easy to do models of them, one reason I like LOC

When revolved it looks like this:

 

[NTP2]

An ogive or as we use it for rocket nose cones a tangent ogive is just a circle segment in cross section.

In Solidworks I use the revolve command and draw a half cross section of the outline as shown below.

View attachment 620385
The R66.43 is the ogive part of the sketch. The important part is that the center point of the circle is located on the vertical hatched center line. This makes the circle tangent to the body tube. For a ogive that is not tangent you can locate the center point of the circle anywhere needed. I put a little .25 radius on the nose to make it more accurate to the actual part but this is not necessary. This particular nosecone is a model of the LOC 7.5 nosecone.
LOC gives dimensions for a lot of their parts, making it easy to do models of them, one reason I like LOC

I am doing a tail cone but same thing basically.

 

[Rschub]

Yup, just cut it off at the diameter you need for the motor tube.

This tailcone is a tangent ogive to the body tube and tangent to the straight tapered end.

 

[NTP2]

Yup, just cut it off at the diameter you need for the motor tube.

This tailcone is a tangent ogive to the body tube and tangent to the straight tapered end.

View attachment 620387

One question how do you find the size of the circle? All I have is the 2 lines that I need to connect?

 

[Rschub]

One end of the circle starts at the end of the body tube and is tangent to it. The radius of the circle depends on the length of the curve you need, in my drawing above it was 28 inches. The circle sizes itself if you have the length dimension set. The circle segment should be snapped to the end of your line.
In Solidworks you can do a 3 point arc, there should be something similar in F360.

 

[NTP2]

One end of the circle starts at the end of the body tube and is tangent to it. The radius of the circle depends on the length of the curve you need, in my drawing above it was 28 inches. The circle sizes itself if you have the length dimension set. The circle segment should be snapped to the end of your line.
In Solidworks you can do a 3 point arc, there should be something similar in F360.

Ok a see, thanks!

 

[dr wogz]

Sketch constraints!


learn them love them, use them!

same with work planes, work points, and work axises

 

[Sandy H.]

Sketch constraints!


learn them love them, use them!

same with work planes, work points, and work axises

I've had the unfortunate experience of needing to use CATIA quite often. Of course, no training and self taught with the help files (Frenglish) and forums. For me, if I can't seem to figure out how to do something in CATIA, my go-to is to add work points. In Inventor, I rarely add workpoints.

I think CATIA is an amazingly powerful piece of software, but I really think one needs to have real training, do a bunch of work and then go back to training. Inventor was pretty easy to self-teach. In Inventor, I feel like adding workpoints means I didn't do my job up front, while in CATIA it is a requirement. Work planes in Inventor are absolutely a great tool, though.

I think Solidworks might be in the middle of CATIA and Inventor as far as features and workflow. Ironically, I did get a 1 week training on Solidworks, but never had a project to do using it afterwards, so I'm completely an amateur on the one piece of software I was trained on vs. the other two that I use often with no training. . .

For the OP, though, I'd say watching a bunch of videos can help get acclimated to the software, but getting the mindset of how to build a part is very critical for knowing how to start sketches etc. I came up working with my hands and running machines. I was in a very subtractive environment (i.e. take a round bar and remove material on the lathe etc.). I think it is helpful to envision the manufacturing process during the design process and to model in a similar manner. If you're working in an additive manufacturing environment, maybe build stuff up in bits, but if your in a subtractive environment, start with a big round bar and cut it the same way the guy in the field would do it. Not sure I'm right in that belief, but I'm old enough to be stuck in my ways, so that's how I look at it.

 

[NTP2]

For the OP, though, I'd say watching a bunch of videos can help get acclimated to the software, but getting the mindset of how to build a part is very critical for knowing how to start sketches etc. I came up working with my hands and running machines. I was in a very subtractive environment (i.e. take a round bar and remove material on the lathe etc.). I think it is helpful to envision the manufacturing process during the design process and to model in a similar manner. If you're working in an additive manufacturing environment, maybe build stuff up in bits, but if your in a subtractive environment, start with a big round bar and cut it the same way the guy in the field would do it. Not sure I'm right in that belief, but I'm old enough to be stuck in my ways, so that's how I look at it.

This is going to sound arrogant but, I already thought of that I have been thinking about how a machinist will make the parts from almost day 1 it’s just how I thought you were supposed to do it.

 

[GlenP]

I don't suppose anyone knows how to do an ogive curve? google was not helpful.

https://en.wikipedia.org/wiki/Ogive

 

[NTP2]

https://en.wikipedia.org/wiki/Ogive

Thanks but I have got it figured out already…

 

[dr wogz]

This is going to sound arrogant but, I already thought of that I have been thinking about how a machinist will make the parts from almost day 1 it’s just how I thought you were supposed to do it.

not quite. You can design to meet a bunch of design criteria; machining is but one 'need'.

ideally, you need to design / draw the part so it is easily editable later on. "simple & fastest isn't always the best approach.. All parts get revised at some point. The 'knack' is know what will likely change in the future.. It may take an extra 20 minutes, and have a few extra features, but when that change is needed, you no longer then have to 'redraw the part', but only edit a feature or two.. (And other constraints & design / assembly aspects are kept..)

and remember as well, that the drafting is a language, and you need to design / draw accordingly.. that way, the drawing can truly follow the part. (your placed dims on the part should be the dims you use on the dwg..)

 

[GlenP]

Thanks but I have got it figured out already…

I guess sarcasm is hard to convey on the internet, but arrogance comes across loud and clear!

 

[Bravo52]

...ideally, you need to design / draw the part so it is easily editable later on.

This!

That is the Raison d'être of modern CAD software. Parametric design is the "game changer" as they say.

 

[dr wogz]

The next step in 'CAD knowledge' is knowing how to put assemblies together. knowing what are the logical sub assemblies is key to keeping things (model tree) nice, neat & tidy. Also, knowing how to make the assembly 'common' so that you can use it over multiple assemblies.

make sub assemblies that make sense, and (should) follow manufacturing / assembly process on the shop floor.

The example given (the HoJo) make the motor mount a sub-assembly. You can then pull this sub-assembly into other designs, and you no longer need to assembled (and explode) those 4-6 parts each & every time (and that sub assembly allows you to create one graphic, that can be used in multiple instruction sheets, further saving time & resources..

and I can go on..

 

[NTP2]

I guess sarcasm is hard to convey on the internet, but arrogance comes across loud and clear!

It’s not arrogance if you look at how long it took me to figure it out, even with very good advice.

 

[kramer714]

@jackiboi_11 I have your rail guide! Just epoxy to the tube, it's for a 1-inch rail.

good start... but now think about how you can improve it. That is the beauty of cad, once you have the parts of the model you can, add, edit etc. I took yours and added a few things, some of the features are easy to add, some more difficult. You should be able to take the step file and play with the features.

Some things that would be helpful on a rail guide,

• Features to maintain bond line (i have .2mm bond line standoff - 4 plcs)
• Attachment holes (good for installation to keep the lug from moving), this is sized for small countersunk aluminum rivets, just needs final drilling of hole. Small screw works too.
• Fairing, Filleting, Chamfering the edges.
• Notch for aligning to a scribe line.
• peel stoppers (grooves on the bond surface)

Plus I gave you a model with just the surfaces.

Fun eh?

Mike K

 

[kramer714]

The next step in 'CAD knowledge' is knowing how to put assemblies together. knowing what are the logical sub assemblies is key to keeping things (model tree) nice, neat & tidy. Also, knowing how to make the assembly 'common' so that you can use it over multiple assemblies.

make sub assemblies that make sense, and (should) follow manufacturing / assembly process on the shop floor.

The example given (the HoJo) make the motor mount a sub-assembly. You can then pull this sub-assembly into other designs, and you no longer need to assembled (and explode) those 4-6 parts each & every time (and that sub assembly allows you to create one graphic, that can be used in multiple instruction sheets, further saving time & resources..

and I can go on..

Yeah, Agree,

One of the first things I had a SLI team i was working with was to create a BOM (Bill of materials) indented to show the 'goesinta', what PART goesinta what sub assemblies, and what sub assemblies goesinta what final assemblies.

This helps prioritize what needs to be done first, how the tolerances stack up, and a way of keeping track of the release status. Each part / sub assembly got its own part number, dashes show sub assemblies. Old school configuration management but it still works.

 

[dr wogz]

Yeah, Agree,

One of the first things I had a SLI team i was working with was to create a BOM (Bill of materials) indented to show the 'goesinta', what PART goesinta what sub assemblies, and what sub assemblies goesinta what final assemblies.

This helps prioritize what needs to be done first, how the tolerances stack up, and a way of keeping track of the release status. Each part / sub assembly got its own part number, dashes show sub assemblies. Old school configuration management but it still works.

i do that every day!

i am a BOM technician!!

 

[Rschub]

i do that every day!

i am a BOM technician!!

If you see me running, there must be donuts in the break room.

 

[dr wogz]

If you see me running, there must be donuts in the break room.

our donuts usually get passed around...

wait... let me re-phrase that..

the bringer of donuts usually goes around offering..

 

[c0c0m0ke]

I want to practice CAD, and thought that maybe some of you need a custom part but don’t know CAD? I can do it for you and this is the best part for FREE. The part you should be wary of is that I am very much learning and results may vary. Just send me a PM of what you want.

 

[c0c0m0ke]

I uploaded pictures of 3 rockets I have built or started to Build but have encountered problems. My recovery system needs tuning up. Six color rocket, 29mm motor mount ruptures at ejection. How do I reinforce tube to withstand inner pressure from blowing out the sides. I have thought inserting long couplers or wrapping with Kevlar thread and epoxy, but I am dubious how effective that may be. I have never glassed a tube.

Open for discussion.

Carlos