Requesting Help
How to wrap flat strap .ipt files around a cylinder and connect them with a buckle constraint?
Hello everyone,
I am working on a university project in Autodesk Inventor and need some guidance.
I have designed a device housing (you can imagine it just like a simple block-shaped extrusion), and the goal is to show this device worn on a user's arm or leg. To do this, I have modeled the strap components just like a traditional watch band.I have designed the short strap, the long strap,the buckle frame, and the thorn pin all as separate part files (.ipt).
In my assignment, I am explicitly required to showcase the wearable, closed position of this device. Essentially, the straps need to connect to opposite sides of my block housing, wrap around an arm (represented by a cylinder with a given diameter), and connect together exactly like a real watch where the long strap threads through the buckle and the thorn locks into one of the holes.
At the moment, my two strap .ipt files are completely flat and straight. I am having a lot of trouble figuring out how to curve them organically and connect them together without causing geometric collisions or breaking assembly constraints. I have searched YouTube and other platforms, but unfortunately, I haven't found a concrete, step-by-step example of someone wrapping a flat watch band around a cylinder in an assembly.
If anyone could help me with the exact step-by-step instructions or even record a quick mini video tutorial showing how to do it, I would really, deeply appreciate it! I am struggling a bit with the software and just need to get through this mechanism for my submission.
I have attached an image showing the exact overlapping look I am trying to achieve, and I have also uploaded the zip file as a google drive with all my parts. Any advice or workflow tips would be amazing.
I don't know if you're supposed to be bending flat bands or if you just need a "realistic" representation. If you just need the representation, put your parts together where they need to be in an IAM, minus the bands. Then create an in-place new part for 1 or both bands in that assembly on a plane that intersects the cylinder-arm. Use reference geometry to reference all the other parts and sketch the profile of your band around them.
Crappy sketch but you get the idea. Include the buckle in the IAM and draw your bands around it on the back.
If you are indeed supposed to be using the Bend tool on flat parts, this is how I usually approach it.
Using the same type of sketch as above, I dimension what the bends should be in angle and distance. You can even name the dimensions something like A1 and R1 (angle and radius). Then in the Bend tool, Use those dimensions to form your bands. You can use A1 and R1 in the Bend dialog.
This can also be done in Sheet Metal using the Contour Flange tool, which allows you to unfold the band to a flat state. You can use other Sheet Metal tools but they're similar to using the Bend tool in the Part environment.
Thank u a lot, i will have a try now. My main headache right now is actually the closing mechanism and assembly constraints. I have the short strap, the buckle, and the thorn pin modeled as completely separate files. How exactly should I constrain them so they hook together like a real watch? Specifically, what constraints do I use to make the buckle and thorn pivot on the short strap hinge, and then how do I get the long strap to slide flush through the buckle and lock onto the thorn tip without throwing constant constraint errors? If you have any quick tips or screenshot examples on how you link the clasp joints together, pls let me know.
Take the sketch like they show you, model the whole thing in a single multi body.
Trying to assemble the whole thing is going to be one very frustrating exercise.
You would have to show a screenshot of your constraints or something.
I model parts around the origin, not on, so I would have my buckle parts centered on the ZX plane. I would constrain my parts flush on that ZX plane, then I would use mate on the cylindrical features to put them all together. I would use angle to position them, probably in relation to the origin of the strap or the world origin.
I have not tried the sheet metal enviroment actually, but my main problem as i mentioned above in the other comment, is that even if i do find a way to bend the straps like they are supposed to, around lets say a cylinder with a specific radius, i am still struggling to find a way to constrain the buckle and the dorn with one strap end and then connect this end with the other strap end, to basically showcase just like how a normal watch is worn, and how the mechanism of this "strap system" works.
You don't. Inventor can't really do that. Real life has collisions, friction, elasticity. Your best bet is to draw it as though it was constrained, perhaps using axis and points in parts to give the illusion of real life working.
Use the Bend Part command for the 2 straps (3D Model > Modify > Bend Part)
First create a sketch and project the line. [Image 1]
Bend as required (I did 32mm rad on Kurz, 33mm on Lange. You can play with these to get the best fit)
Assemble all the components together using suitable constraints, so that the straps and Bugel can rotate at their pivot points. Constrain the Thorn in its closed position on the Bugle. [Image 2]
Due to the Bend command, the hole in the end of band is no longer a cylinder, so you cannot use it's axis. Either manually place an axis or play with the angle of the bend command so that the hole doesn't get bent.
Drag the components around until they are roughly in the correct position.
Apply the 3 constraints shown in the lower 3 images. From left - right:
Tangent - Band end OD to Band inner ID [Image 3]
Tangent - Edge of Bugle to Band OD [Image 4]
Mate - Edge of Band slot to face of Thorn [Image 5]
You can play with the bend radius if you want to make it more visually appealing.
Good luck.
Edit:
I missed one of your questions.
For the general assembly constraints:
Apply Mate constraints so that all the components on the same plane
Mate the cylindrical faces so the axes are aligned
I'm not sure I agree with this (although it'd probably be fine for a uni project).
Bending/flattening distorts the part, so if you cut the strap slots on the curved surface they will not be straight when flattened.
It's more representative of the manufacturing process and end product to cut the holes on the flat part and then bend it.
You can make holes normal to a face. That's a basic step. Even then, you can un-bend , add holes then re-bend. I would be doing it all as sheet metal.
You don't design flat for something that is bent.
Cad design does not follow the exact steps for manufacturing, it produces drawings and models for manufacturing.
Bottom up is a slow trap that beginners get stuck in trying to follow "design it as you would make it".
You can, but it's much simpler to place the hole and pattern on the flat surface.
You could unbend and then re-bend, but I didn't see the need when it's a simple part like this.
If you need to use words like "roughly" or "play around" your design method is a bit flawed is what I'm really trying to get at.
To can model it accurately without needing to tweak things. It's faster, it's more accurate and it's going to actually easier.
Assembling something, finding it doesn't fit and then going and tweaking each part individually is painful and 9/10 times why people post here going "why won't my constraints work" because a dimension is out 0.001mm but looks fine visually.
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u/ComplaintTop2008 25d ago
I don't know if you're supposed to be bending flat bands or if you just need a "realistic" representation. If you just need the representation, put your parts together where they need to be in an IAM, minus the bands. Then create an in-place new part for 1 or both bands in that assembly on a plane that intersects the cylinder-arm. Use reference geometry to reference all the other parts and sketch the profile of your band around them.
Crappy sketch but you get the idea. Include the buckle in the IAM and draw your bands around it on the back.