Table-Top or Toolpost Shaper

Here's a "working" concept of a small shaper. The design goal is for it to work in the lathe via a toolholder in the toolpost or, on a small table-top fixture. The main use will be for cutting fairly small keyways in pulleys or gear bores. I'm also using this project to learn Fusion 360 after many years of Alibre CAD.

The design is based on the classic Whitworth "Quick Return" slider/shaper mechanism. This is the first time I've used a CAD program for all the conceptual diagrams. I did not use a pencil or notepad for hand sketches like I usually do. I used pencil/paper only for a handful of trig problems and also to calculate the position, torque and speed of the slider rod given the small gear motor that was selected for the project.

This diagram is no-where near what it will finally look like. This diagram only shows the mechanical model to prove-out the basic design. My design goal was to have a shaper that had an adjustable stroke up to 3.25". Fusion 360 has stress analysis and simulation abilities and this conceptual model was used to verify the range of motion and stress areas. The computer model actually "works", in that the motor shaft can be turned and all members move accordingly. It was a fun little project to learn Fusion 360.

For reference, in this model, the slider rod is 8.5" long. The block that holds the slider is theoretically pinned in this model as is the motor and the plate that the assembly is mounted on.
Shaper Concept.JPG

The gear motor will be here in a couple weeks along with a fresh supply of small bearings. I'll work on the model until I'm happy with the "final" design and then I'll build it. Most of the components you see are in their final form but, the enclosure, clapper box and self adjusting mechanism is not even started yet. That will be pretty cut-and-dry.

I'll post a few more pictures at various milestones as things progress.

Ray
 
Bob,

First and foremost, I'm glad your wife is back on her feet. Wow. That's a lot to go through. Learning Fusion 360 can wait, given the circumstances. Fortunately for us, this place is called "Hobby" machinist and we get to prioritize these activities any way we want. If you decide to jump into it, sure; I can help -or at least try to help...

Ray
Thanks Ray.
 
I consider myself moderately skilled in CAD. I really, really like Fusion 360, but I can't figure out why Autodesk did what they did with components and the history. It just isn't that intuitive. I think a couple more of Lars' videos and some more projects might make it click. Gotta stick with it I guess!

Really looking forward to seeing this project come together! Thanks Ray!


Bryan / All,

I'm re-making the parts from the concept model from above and started with the motor drive arm and clamp.

The parts here are very simple but I spent several hours trying to learn the fine points of Fusion 360. I think it was time well spent.
These are the parts that allow an adjustment to change the overall throw-distance of the slider arm. They are more complicated than need-be but, this is an exercise in learning Fusion 360 and showing how the small parts will be made.

These three parts were made separately but, the clamp is made from a projection of the arm. No explicit dimensions are carried between the two so, if one sketch is changed, the extrusion on the other will auto-adjust.

The clamp was created as a single body then split into two pieces. Even though they are different, I decided to leave them in the same component folder.

When doing a series of steps on either of the components, you can switch back/forth between them and move the history elements around and group them. Also, I found that if adjustments are needed on a sketch or extrusion, just grab it from the timeline and select edit. This keeps the number of history point to a minimum. I discovered if you have a bunch of move operations, you can usually delete all but one and condense all the moves into one operation. Make as many as you need as you go but in the end, summarize them into just one or two.

DriveArmAndClamp0.JPG

Two long series of history elements were created from a long series of step while working on both parts simultaneously (see the red boxes). When I made these parts, the series of operations were scrambled into 1 timeline. The exercise I embarked on was to see if the timeline can be re-organized after the fact. It's possible!
DriveArmAndClamp2.JPG

Once it was streamlined, each string of history elements were put into their own group and it condenses the timeline nicely.
DriveArmAndClamp1.JPG


BTW: The mouse can move the clamp on the arm but, I did not set realistic mechanical stops or limits. Next, I'll take a stab at making 2D drawings. That will be a new thing to learn in Fusion 360 and I'll show them when done.


Finally, it will be time to make the real part which I'll work on this weekend if all goes well.

Ray
 
Last edited:
@Ray C Not sure if you're aware, but in any case, don't forget that you can move thru the history to a specific point if you need to make edits or other changes. Helps to keep the timeline from becoming a hopeless mess. You also mentioned keeping some parts together inside a component. did you know that you can group components inside another, empty component? This top component then becomes an assembly containing the components you created or moved inside it.

Also, it's good to name everything. the component, sketches, bodies et al should have similar names so that when you mouse over the history timeline, you know what you're looking at. Helps a lot.
 
These three parts were made separately but, the clamp is made from a projection of the arm. No explicit dimensions are carried between the two so, if one sketch is changed, the extrusion on the other will auto-adjust.

The clamp was created as a single body then split into two pieces. Even though they are different, I decided to leave them in the same component folder.

When doing a series of steps on either of the components, you can switch back/forth between them and move the history elements around and group them. Also, I found that if adjustments are needed on a sketch or extrusion, just grab it from the timeline and select edit. This keeps the number of history point to a minimum. I discovered if you have a bunch of move operations, you can usually delete all but one and condense all the moves into one operation.

Ray, thanks for the write up and explanation. Youtube videos are great, but they lack the context only the written word can express and you do an excellent job on that front. This makes a little more sense now. I'm struggling with the one component based on another component problem. I'll have to come back to this post for reference in the future.
 
Here's a first crack at some 2D drawing to take into the shop. These were made after watching a YouTube video followed by jumping in and cranking them out. Very easy to do. These are NOT high professional quality in terms of what a draftsman could produce but, this is just perfect for my purposes. With a little more editing time, I could add tolerances and get all the images perfectly lined up etc. This was just a first pass at doing this. It's much easier to do in Fusion 360 than in my old CAD program.

Drawing1.JPG
Drawing2.JPG

Drawing3.JPG
Drawing4.JPG

@MikeWi: Thank you... Oh yes, I've been playing around with so many different features and tricks, it's really hard to remember them all. I just need a lot more practice.

Also, I did make sub-components but, had to explicitly bring them to the top level because they would not show-up as individual table elements in the 2D drawings.

FYI: I'm just posting images of the drawings for now. There is a PDF export feature but, it's including PII from the license/registration in the metadata.

Ray
 
Isn't it interesting how the producers of a tool get to control the mental and physical processes of the user/craftsman/artist/engineer/designer.

I was lucky enough to have access to ProEngineer in my career and became a fairly proficient user before I retired in 2003. At my initial introduction to ProE (early '90s) I found the user interface to be, for the most part, intuitive. Case in point, there were "parts" and there were "assemblies". That is a paradigm that I understood without reeducation. It seems to me that the basic paradigm didn't need modification by renaming "parts" as "components" and allowing assorted parts to exist in a single "component" with the resultant potential for complexity of user discipline and/or model modification.

How does the ability to model multiple parts within a single "component" enhance the design development and documentation process?
 
Also, I did make sub-components but, had to explicitly bring them to the top level because they would not show-up as individual table elements in the 2D drawings.
Ray
That's strange, if you mean that the components aren't shown in the part list table? Works for me. I don't know what would cause it though.
 
Isn't it interesting how the producers of a tool get to control the mental and physical processes of the user/craftsman/artist/engineer/designer.

I was lucky enough to have access to ProEngineer in my career and became a fairly proficient user before I retired in 2003. At my initial introduction to ProE (early '90s) I found the user interface to be, for the most part, intuitive. Case in point, there were "parts" and there were "assemblies". That is a paradigm that I understood without reeducation. It seems to me that the basic paradigm didn't need modification by renaming "parts" as "components" and allowing assorted parts to exist in a single "component" with the resultant potential for complexity of user discipline and/or model modification.

How does the ability to model multiple parts within a single "component" enhance the design development and documentation process?

At every level, the tools employed impact any given situation. This is why there are at least 5-10 CAD programs in the top tier (with the mother of them all probably being Catia -which is used for battleships, ocean liners, 747's, nuclear power plants etc) another 25 in the second tier and another 50 in the third tier. I'm making those numbers up. There are probably way more than 100 CAD programs out there. You get to pick what works best for you. BTW: I've encountered the same thing with different modeling languages. Almost always, the constructs and syntax of the language impact the design.

Alibre for example is (in my opinion) semi-parametric. You make parts in separate files then assemble them in a different file. If you want to share one particular dimension in 2 different parts, you need to define a named parameter and put it in a global dimension file. If you change that dimension, you need to visit each part and rebuild it. At times, this method of doing things has driven me to the brink of insanity. In Fusion, all the parts of an assembly are (usually kept) in one file, each kept inside a component. The component has all the sketches. If you want to share a dimension across multiple parts, you pull-up the associated sketch and project that dimension into the sketch for that other part. (BTW: You can do this in Alibre but, it's not at all easy to do and has many restrictions about which constructs can be projected). If you re-draw one of the parts that uses that dimension, everything automatically rebuilds. Actually, though, in Fusion, you can also optionally define a table of global parameters -so you can take either approach or, mix the two.

Keeping one part as a sub-component of another has a lot of advantages. In my case, I split something in half. I drew the whole thing with one sketch then split it. Both of the halves fit perfectly and if I tweak one, the other automatically changes. Since they are related and tightly coupled it makes perfect sense to keep them grouped for easy reference and retrieval.

... The CAD program that's best for you, is the one that suits most of your needs and is easy for you to use. Way back when, I was testing different CAM programs. The best I can say about that is I hated some less than others.


Ray
 
That's strange, if you mean that the components aren't shown in the part list table? Works for me. I don't know what would cause it though.

Yep, that's exactly what happened. It could be a bug but, very likely it's operator error. No worries. I dragged it out one level, re-created the sketch and bingo... All 3 parts showed-up in the table. I can fiddle with it later and figure it out.


Ray
 
Back
Top