Parametric CAD slipjoint tang

[Signalprick]

I guess the broader point is that CAD can certainly be a valuable tool to help understand and build slip joints but I can't stress enough that you should put your drawings to steel and work a couple out. Then you could truly use your CAD skills to design a better knife because you'll actually know what works and what doesn't.

 

[Hubert S.]

I guess the broader point is that CAD can certainly be a valuable tool to help understand and build slip joints but I can't stress enough that you should put your drawings to steel and work a couple out. Then you could truly use your CAD skills to design a better knife because you'll actually know what works and what doesn't.

I plan to do just that, but have not found the time yet. I did build a surface grinding attachment for the grinder and a rise-and-fall indicator earlier this year and hopefully I'll get around to building a slipjoint soon.

 

[Signalprick]

I plan to do just that, but have not found the time yet. I did build a surface grinding attachment for the grinder and a rise-and-fall indicator earlier this year and hopefully I'll get around to building a slipjoint soon.

Good deal! It can be challenging but so much fun. Looking forward to seeing your progress. Since you mentioned Chris Crawford's site I'll just say this, the Swenson video is a priceless reference. The Ruple and the Brewer are good too but the Swenson I think is the most in depth for a beginner. Worth every penny and then some. Can't recommend it enough.

 

[BradleySmall]

I think you can eliminate the "hand-waving and a little magic" with my process. I am not sure if there is a simpler way to do it, you have to find the intersection of two lines somehow. I'm very interested in what you come up with. The only reason I even tried this in CAD is the protruding tang in the pictures you posted in the other thread. I cannot imagine that will make for a smooth operation, that's why I thought it should be constrained.

I would be happy to work together with you to come up with something. I am not 100% sure I understand your specific concern?

 

[Hubert S.]

I would be happy to work together with you to come up with something. I am not 100% sure I understand your specific concern?

It just looks odd to me, might well be my lack of understanding or imagination. At some point during the rotation, the two corner points must touch if the tang is proud and it is not clear to me where the force vector between the two would point at that instance since the normal vector for both surfaces is undefined at the discontinuity. If the corner of the tang is on the other side, the force vector is perpendicular to the spring (if there is no friction), so the force is always in the direction you want it to be. It is probably not an issue once you round the corners a bit.

 

[BradleySmall]

It just looks odd to me, might well be my lack of understanding or imagination. At some point during the rotation, the two corner points must touch if the tang is proud and it is not clear to me where the force vector between the two would point at that instance since the normal vector for both surfaces is undefined at the discontinuity. If the corner of the tang is on the other side, the force vector is perpendicular to the spring (if there is no friction), so the force is always in the direction you want it to be. It is probably not an issue once you round the corners a bit.

That sounds the way I understand it

 

[BradleySmall]

It just looks odd to me, might well be my lack of understanding or imagination. At some point during the rotation, the two corner points must touch if the tang is proud and it is not clear to me where the force vector between the two would point at that instance since the normal vector for both surfaces is undefined at the discontinuity. If the corner of the tang is on the other side, the force vector is perpendicular to the spring (if there is no friction), so the force is always in the direction you want it to be. It is probably not an issue once you round the corners a bit.

Okay, so I took a look. I put one single value into a spreadsheet and for lack of imagination or the ability to think of a better name, I called it "Unit". You would't think I was a Software engineer for over 30 years, I might be able to pick better variable names than I do... but there you have it. Other than the 3/32 pivot hole, everything else is based on that value, either 2x 3x 4x etc... Even the curves. I put some fillets on the pointed corners and things look really good, but I removed them because it added far too much complexity to the base constrained concept piece.
The only other numeric value I used was 8° to handle the 172° closing angle and I simply hard coded that into place. Oh, yeah, I gave the back square a 2° relief angle, and the end of the spring a 1° relief. But everything else was either geometric or based on the "unit". It scales really well now. I did use some construction lines to hold some stuff together, but it pads out nicely, and rotates quite well. I am still not good at doing the round choils, seems like 3 or more arcs in some funny directions and with some weird groupings of coincidence and tangents, but I am leaving that as an exercise in itself. Or shall I say "an exercise for the reader" as they so like to do in text books for things they don't feel like explaining, or don't really know the answers to. Kind of like implementing self balancing trees without recursion

I am using a shape binder to manage the spring, so if you'd like to try out the fillet tool on those pointy corners, be very careful or you will really hurt yourself on the spring. They call one of them "constraint preserving" but it's a lie It will change the number of edges, and the edges that the shape binder is using will change and it will do all sorts of wacky things to your spring. You've been warned, and forewarned is forearmed!

"justthetang" for FreeCAD version 0.20

Here is the link to it in my DropBox, hopefully I shared it correctly. Let me know otherwise. I have more trouble sharing files here on this web forum. Perhaps it would be easier if I paid or something. But it is what it is.

 

[BradleySmall]

It just looks odd to me, might well be my lack of understanding or imagination. At some point during the rotation, the two corner points must touch if the tang is proud and it is not clear to me where the force vector between the two would point at that instance since the normal vector for both surfaces is undefined at the discontinuity. If the corner of the tang is on the other side, the force vector is perpendicular to the spring (if there is no friction), so the force is always in the direction you want it to be. It is probably not an issue once you round the corners a bit.

Just since you are the only one that has shown much interactive communication on FreeCAD with me, I thought you might like to see this one as well. It is a ToothPick, that I worked with after fixing up some very unacceptable Inkscape SVG then imported it into the Draft, then Sketcher/Part Designer. But you might find it interesting how I used the subtractive cone to do the nail nick, and the subtractive pipe to give it a hollow grind.

I haven't added the frame/liner/scales to it yet, but that wasn't the goal at the time.

svgImportToothpick - FreeCAD 0.20

I'll be interested to hear even if it just opens for you

 

[Hubert S.]

Okay, so I took a look. I put one single value into a spreadsheet and for lack of imagination or the ability to think of a better name, I called it "Unit". You would't think I was a Software engineer for over 30 years, I might be able to pick better variable names than I do... but there you have it. Other than the 3/32 pivot hole, everything else is based on that value, either 2x 3x 4x etc... Even the curves. I put some fillets on the pointed corners and things look really good, but I removed them because it added far too much complexity to the base constrained concept piece.
The only other numeric value I used was 8° to handle the 172° closing angle and I simply hard coded that into place. Oh, yeah, I gave the back square a 2° relief angle, and the end of the spring a 1° relief. But everything else was either geometric or based on the "unit". It scales really well now. I did use some construction lines to hold some stuff together, but it pads out nicely, and rotates quite well. I am still not good at doing the round choils, seems like 3 or more arcs in some funny directions and with some weird groupings of coincidence and tangents, but I am leaving that as an exercise in itself. Or shall I say "an exercise for the reader" as they so like to do in text books for things they don't feel like explaining, or don't really know the answers to. Kind of like implementing self balancing trees without recursion

I am using a shape binder to manage the spring, so if you'd like to try out the fillet tool on those pointy corners, be very careful or you will really hurt yourself on the spring. They call one of them "constraint preserving" but it's a lie It will change the number of edges, and the edges that the shape binder is using will change and it will do all sorts of wacky things to your spring. You've been warned, and forewarned is forearmed!

"justthetang" for FreeCAD version 0.20

Here is the link to it in my DropBox, hopefully I shared it correctly. Let me know otherwise. I have more trouble sharing files here on this web forum. Perhaps it would be easier if I paid or something. But it is what it is.

It looks pretty good to me. There is some very slight interference in the closed position, but I think it's probably less than the line width you would use for printing the template, so it does not really matter. You can eliminate that if you remove constraint 20 which pins the end point of your 8 degree line on the horizontal line at distance "Unit" below the pivot. Instead, set the length of the line at 8 degrees to "Unit", then it will be correct. This solution is the same as mine, except you have a few more things hard coded. Looking over this, I now think there is an easier way to do this. You can just use a vertical line of length "Unit" and rotate it around the pivot by the closed angle, then add a perpendicular line to the end of it. Do the same for the half stop angle and intersect the resulting two lines. This is probably a bit more intuitive than the way I described above, unless you think about the constraints in a polar coordinate system.

I would add the relief on the spring to the top instead of taking it away from the bottom. That way you can eliminate the slight overhang at the half stop (and closed position if the half stop angle is half the closed angle). Again, this won't matter at all for practical purposes, the error is just over 3 thou for your chosen value of "Unit".

 

[Hubert S.]

Just since you are the only one that has shown much interactive communication on FreeCAD with me, I thought you might like to see this one as well. It is a ToothPick, that I worked with after fixing up some very unacceptable Inkscape SVG then imported it into the Draft, then Sketcher/Part Designer. But you might find it interesting how I used the subtractive cone to do the nail nick, and the subtractive pipe to give it a hollow grind.

I haven't added the frame/liner/scales to it yet, but that wasn't the goal at the time.

svgImportToothpick - FreeCAD 0.20

I'll be interested to hear even if it just opens for you

It opened. The subtractive pipe is pretty neat. I poked around a bit, but then I must have done something wrong and it would not recompute anymore. I'll have to look at it again tomorrow.

 

[BradleySmall]

It looks pretty good to me. There is some very slight interference in the closed position, but I think it's probably less than the line width you would use for printing the template, so it does not really matter. You can eliminate that if you remove constraint 20 which pins the end point of your 8 degree line on the horizontal line at distance "Unit" below the pivot. Instead, set the length of the line at 8 degrees to "Unit", then it will be correct. This solution is the same as mine, except you have a few more things hard coded. Looking over this, I now think there is an easier way to do this. You can just use a vertical line of length "Unit" and rotate it around the pivot by the closed angle, then add a perpendicular line to the end of it. Do the same for the half stop angle and intersect the resulting two lines. This is probably a bit more intuitive than the way I described above, unless you think about the constraints in a polar coordinate system.

I would add the relief on the spring to the top instead of taking it away from the bottom. That way you can eliminate the slight overhang at the half stop (and closed position if the half stop angle is half the closed angle). Again, this won't matter at all for practical purposes, the error is just over 3 thou for your chosen value of "Unit".

Like I had mentioned before, I have a tendency of using construction geometry then throwing it away. So I did so in this case. After trimming all the webbing, I went back and tried to remember what I did to add it back in with this being the result. So my bad on that, but I think I know what you are suggesting. Okay, just tried it and it does seem to make it a little tighter. Great catch!! Thanks!

As for the relief, it is kind of bogus anyway. I may go back and leave it fully square but haven't decided yet. There is so much final fit-up involved, and the accounting for the spring preload and tension issue, that I just as soon have more that I can take off, than less... A bit harder adding more spring It did feel right at the time, because it demonstrates the 2-point-contact concept directly. But otherwise, may be simpler to leave out. The "overlap" at 90° would go away if I filleted the corners, or when I simply round them over with the belt grinder. I also assume that the kick will be rounded a bit and that will smooth it out overall. When cutting out a blank such as this, I would leave the line fat and this would definitely be an area that I want some extra meat for final fitup.

 

[BradleySmall]

It opened. The subtractive pipe is pretty neat. I poked around a bit, but then I must have done something wrong and it would not recompute anymore. I'll have to look at it again tomorrow.

I have found trying to reverse-engineer some of these sheets can get hairy. And remember, i am using .20 so if you are using .19 or .21 it is likely you will hurt yourself if you do anything it thinks is a modification. In another file I used a cylinder in .20 and there they allow you to "tilt" which I would better think called a "skew" but no one asked me... Well, that feature of the cylinder doesn't exist in .19. But it takes a few changes before it misses it, then everything goes to hell

Anyway, I was kind of happy that I was able to use the subtractive pipe much in the way I would a contact wheel to do a hollow grind. If only my hand were as steady as that tool when i get to the grinder.. Goals... right?

So, this was just a short diversion back to the beginning tang design/constraint. In my earlier design I was able to, given spine length, straight edge length, "belly-rise-angle", "point offset from centerline", and a few radii size modifications, I was able to generate blade spine/edge shapes with corresponding spring inner profile shapes. I could do pretty much all the "clip point" and most "clip point like" shapes including spey. This involves an inward curve in the clip area, and by adjusting the radius it can be flattened down to what would look like a "drop point" to the degree that these overlap. However, it looks like I will need a second blade to do true "drop points" such that the drop/clip curves outward. This will be necessary to handle spear point, as well as the sheep and lambs feet, coping, and I think Wharncliff will be manageable with this as well.
I have asked about changing the direction of an arc on the FreeCAD boards, and with one exception, that I am really not quite understanding well, they are not pointing me in a good direction to be able to do that from the spreadsheet. But I think I can handle managing 2 files instead of just 1. That should cover me up to the point where I need to get crazy and add "recurve" or some one-off shape. I am not concerned with those situations yet.

The next really interesting bit is to manage the frames/dies/scales/body shapes. I think this involves some vernacular that either I am lacking, or simply isn't formally agreed upon as of yet. The reason I say that is each level of thing, has a couple variations to go on. Let's say we start off with a cigar, like a kampking. It involves 4 arcs connected tangentally with each opposing radii being equal. There is a ratio between the smaller radii and larger radii that will determine if it is a "ROUND BOLSTERED" pen, camp knife, sunfish/e.toenail, EE jack, or SAK. And somewhere in there is a length vs width that plays along too. However, each of those radii-ratio-length-width have another issue that can come into play in that they can also be a square bolstered, or semi-square bolstered, or round-capped square or semisquare bolstered. Once you allow for unequal ended you get into barlows, and sleeveboards, english jacks, pens and so forth. This is all before you allow the slight rotation of the ends into serpentine, dogleg, swayback, sowbelly, congress, slim, peanut, saddlehorn... not to mention what happens when the toothpick, fish (I think F. Beltrame's stilettos are fish shaped but I digress ).

I have traced many of these from the old catalogs, and the new ones, and anywhere else I can find. That gives me lots of SVG starting points and reference shapes. But, again, like the blade shapes, I want to get to a point where I can parameterize them. But I am not sure what to call everything, or exactly what the interplay should be. Especially going from one bolster shape to another.
If this is an area you have any interest in, I would love some collaboration. As I see it, if it can be defined well enough, and simply enough, and I believe it can. It can enable indexing, and database entries and searches, and other classifications and generation of some really cool and possibly novel designs. I know this may be too nerdy-geeky or "overthinking" to a lot of people. But I would really love to deep dive this, especially if I can find someone else with some amount of interest in it.

 

[Hubert S.]

I have found trying to reverse-engineer some of these sheets can get hairy. And remember, i am using .20 so if you are using .19 or .21 it is likely you will hurt yourself if you do anything it thinks is a modification. In another file I used a cylinder in .20 and there they allow you to "tilt" which I would better think called a "skew" but no one asked me... Well, that feature of the cylinder doesn't exist in .19. But it takes a few changes before it misses it, then everything goes to hell

Anyway, I was kind of happy that I was able to use the subtractive pipe much in the way I would a contact wheel to do a hollow grind. If only my hand were as steady as that tool when i get to the grinder.. Goals... right?

So, this was just a short diversion back to the beginning tang design/constraint. In my earlier design I was able to, given spine length, straight edge length, "belly-rise-angle", "point offset from centerline", and a few radii size modifications, I was able to generate blade spine/edge shapes with corresponding spring inner profile shapes. I could do pretty much all the "clip point" and most "clip point like" shapes including spey. This involves an inward curve in the clip area, and by adjusting the radius it can be flattened down to what would look like a "drop point" to the degree that these overlap. However, it looks like I will need a second blade to do true "drop points" such that the drop/clip curves outward. This will be necessary to handle spear point, as well as the sheep and lambs feet, coping, and I think Wharncliff will be manageable with this as well.
I have asked about changing the direction of an arc on the FreeCAD boards, and with one exception, that I am really not quite understanding well, they are not pointing me in a good direction to be able to do that from the spreadsheet. But I think I can handle managing 2 files instead of just 1. That should cover me up to the point where I need to get crazy and add "recurve" or some one-off shape. I am not concerned with those situations yet.

The next really interesting bit is to manage the frames/dies/scales/body shapes. I think this involves some vernacular that either I am lacking, or simply isn't formally agreed upon as of yet. The reason I say that is each level of thing, has a couple variations to go on. Let's say we start off with a cigar, like a kampking. It involves 4 arcs connected tangentally with each opposing radii being equal. There is a ratio between the smaller radii and larger radii that will determine if it is a "ROUND BOLSTERED" pen, camp knife, sunfish/e.toenail, EE jack, or SAK. And somewhere in there is a length vs width that plays along too. However, each of those radii-ratio-length-width have another issue that can come into play in that they can also be a square bolstered, or semi-square bolstered, or round-capped square or semisquare bolstered. Once you allow for unequal ended you get into barlows, and sleeveboards, english jacks, pens and so forth. This is all before you allow the slight rotation of the ends into serpentine, dogleg, swayback, sowbelly, congress, slim, peanut, saddlehorn... not to mention what happens when the toothpick, fish (I think F. Beltrame's stilettos are fish shaped but I digress ).

I have traced many of these from the old catalogs, and the new ones, and anywhere else I can find. That gives me lots of SVG starting points and reference shapes. But, again, like the blade shapes, I want to get to a point where I can parameterize them. But I am not sure what to call everything, or exactly what the interplay should be. Especially going from one bolster shape to another.
If this is an area you have any interest in, I would love some collaboration. As I see it, if it can be defined well enough, and simply enough, and I believe it can. It can enable indexing, and database entries and searches, and other classifications and generation of some really cool and possibly novel designs. I know this may be too nerdy-geeky or "overthinking" to a lot of people. But I would really love to deep dive this, especially if I can find someone else with some amount of interest in it.

I'm generally interested in this, but I don't have a lot of time to dedicate to it at the moment. I really want to make some progress on my DIY Rockwell hardness tester, and of course, find some time to build an actual slipjoint!

Flipping an arc is indeed not easy, maybe impossible in Freecad. I can flip an entire circle without problem, but not an arc. B-splines are no problem though, and you could compute enough control points in the spreadsheet to approximate a circle if you really wanted to, but B-splines might be preferable anyway, as you can vary the curvature along their length. Since Freecad does not appear to like negative values for length constraints, you have to control their coordinates by using a direction vector that you can flip. This is easily done by using an angle parameter that you set to either 90 or -90 degrees.

 

[BradleySmall]

I'm generally interested in this, but I don't have a lot of time to dedicate to it at the moment. I really want to make some progress on my DIY Rockwell hardness tester, and of course, find some time to build an actual slipjoint!

Flipping an arc is indeed not easy, maybe impossible in Freecad. I can flip an entire circle without problem, but not an arc. B-splines are no problem though, and you could compute enough control points in the spreadsheet to approximate a circle if you really wanted to, but B-splines might be preferable anyway, as you can vary the curvature along their length. Since Freecad does not appear to like negative values for length constraints, you have to control their coordinates by using a direction vector that you can flip. This is easily done by using an angle parameter that you set to either 90 or -90 degrees.

As I said, I can live with 2.i have a bunch of projects in the works too including 6 current slipjoints, a paragraph, and getting the rest of my shop set up. Add this to them, and there is always something to work on.

Perhaps you can sounding board for me on some of these concepts.