So I created a double V belt drive using the belt function in SolidWorks. Now after installing the shafts on the pulleys, and the gearbox the belt has to drive, the belts are not on the pulleys anymore. The pulleys are still concentric with the belt, but the belts have shifted to the side. Rebuilding doesn't fix it. How the hell does this happen and how can I fix it?
I attached the whole assembly to this post for those of you who want to have a look.
Arno,
First and foremost, you must constrain your parts. Go through the tutorial on assemblies. It is free. It is built-in to SWX (Go to Help and you will see SOLIDWORKS Tutorials). I recommend going through ALL of them, but at least you should go through the one on assemblies. I think you will solve your problem rather easily.
I know about constraints, I have a few years of experience with Inventor and I think that's what's troubling me. There's a difference in logic and structure between the two programs. To me it seems logical that when you use certain parts to create something with some kind of design accelerator, the thing you create will be constrained to that part. But apparently when you create a belt using two cylindrical surfaces, the belt path is not constrained to the middle of that surface (which would be logical for a belt on a pulley). The path is only constrained to the surface but can move along that surface. If anyone at SolidWorks reads this, consider changing this please?
I solved it by creating two planes on one of the pulleys and constraining the belts to these planes. I suppose this is how it should be done since there is an option for selecting a 'belt plane' when creating a new belt. Bit inefficient if you have to create a new plane for every belt and can't just use the groove of the pulley, especially when working with multi-groove pulley setups. But anyway, problem solved!
Arno Goossens wrote:
I know about constraints, I have a few years of experience with Inventor and I think that's what's troubling me. There's a difference in logic and structure between the two programs. To me it seems logical that when you use certain parts to create something with some kind of design accelerator, the thing you create will be constrained to that part. But apparently when you create a belt using two cylindrical surfaces, the belt path is not constrained to the middle of that surface (which would be logical for a belt on a pulley). The path is only constrained to the surface but can move along that surface. If anyone at SolidWorks reads this, consider changing this please?
I solved it by creating two planes on one of the pulleys and constraining the belts to these planes. I suppose this is how it should be done since there is an option for selecting a 'belt plane' when creating a new belt. Bit inefficient if you have to create a new plane for every belt and can't just use the groove of the pulley, especially when working with multi-groove pulley setups. But anyway, problem solved!
Please post your solved assembly. Perhaps we can make some suggestions to improve the technique.
Here's the updated assembly!
Arno Goossens wrote:
Here's the updated assembly!
Okay, here is what I found and these are things you should embrace in order to improve your modeling skills:
1. Pulley_Small: First feature has two circles in the sketch, but only one is used for the feature. Cut-Revolve1 has underdefined sketch elements - THIS IS VERY BAD! Make the angled sides symmetric about a center line emanating from the midpoint of the root line segment and they will be properly constrained. This whole part could have been more easily made in one feature, a Revolved Boss that correctly defines the profile such as this.
Note in the image above the centerline of the left groove is coincident with the origin. This conveniently puts an already existing principal plane in the center of this groove, which makes later construction of the belt very easy by selecting this plane. Also note that the right hand groove uses parallel, collinear and equal length sketch constraints. This is so that you only have to make changes to one groove and it will be reflected in the other. Duplicating dimensions is just a recipe for disaster since there are multiple dims that have to be updated and this is often easily missed.
The large pulley has similar problems.
2. On both pulleys it is good to put a sketch on a plane through the center of one of the grooves that only has a circle. This circle should be the pitch diameter of the pulley. Label it as such for later use in making the belt.
3. Your assembly model is floating in space. Fix or otherwise fully constrain something like the box bottom. Just grabbing and moving anything in your assembly messed everything up. This is easily avoided if the assembly is anchored and everything is properly constrained.
4. In reality belts are fixed length, therefore it is a better practice to make the belt part definition a driving length. Leave both pulleys free to rotate and give one of the pulleys a freedom to change its center distance, perhaps constrain the axis of the small pulley to move in an adjusting slot. When you use the fixed length for the belt SWX will automatically move the pulley where it needs to go to satisfy all the parameters.
Normally I would not put this much time into a student project such as yours, but you indicated you have experience with another CAD system so I felt it important to try to help you improve your path in 3D modeling in general and SWX in particular. You are a student and just learning, but that is why it is so important to heed this advice now and make good habits from the start:
ALWAYS make your sketches fully defined.
Make your models efficiently with few features.
Make good use of sketch constraints such as mentioned above.
NAME YOUR FEATURES ON CREATION - this is especially important if your model will have a lot of features, but even more important if someone else will be using your model and needs to understand/change it.
Please accept my comments as helpful and constructive input. I am only trying to shorten your learning curve to prevent frustrations with your modeling.
Also, you really would benefit from carefully going through the tutorials.
Dennis,
Thanks a lot for all that information!
I know about the underdefined sketches, but I couldn't figure out how to properly fully define them. Thanks for showing the centerline thing!
The messy structure is because the pulley had a totally different shape before. Didn't really think much of it, but you're right, less is more. I think I'm just going to completely rebuild the parts and assembly. I need to update some other stuff and make these parts linked to a design table.
About the duplicated dimensions: would having both dimensions linked also be a good solution? I tried to link a few duplicate dimensions using the 'link values' option.
Anyway, thanks again for the feedback!
Arno Goossens wrote:
Dennis,
Thanks a lot for all that information!
I know about the underdefined sketches, but I couldn't figure out how to properly fully define them. Thanks for showing the centerline thing!
The messy structure is because the pulley had a totally different shape before. Didn't really think much of it, but you're right, less is more. I think I'm just going to completely rebuild the parts and assembly. I need to update some other stuff and make these parts linked to a design table.
About the duplicated dimensions: would having both dimensions linked also be a good solution? I tried to link a few duplicate dimensions using the 'link values' option.
Anyway, thanks again for the feedback!
I use Link Values also, but usually for situations where sketch constraints don't work. For instance, where a dimension in one feature needs to be the same value as another on a different feature. Think of sheet metal, where you want some dimension to match the thickness. Linking is very appropriate for this situation. However, in a sketch my rule of thumb is if the entities have something in common then give them those sketch constraints, i.e., line segments (such as the OD of the pulley in the image I posted) that are collinear should be made collinear. Oh, they are equal in length too? Well then let's just give them that constraint as well. The V-grooves are identical so it is so much cleaner to just dimension one and make the other one identical. There are a couple of ways of doing this, including mirroring one groove about a centerline emanating from the center of the line segment between them. You can even make sketch elements constrained to sketch and feature edges outside of the sketch you are working in.
Yes, you could dimension these features twice and link them to their partner, but I found this ends up taking more time than adding the sketch constraints. Besides, if the duplicate dimensions are not needed on the drawing then they would just add a lot of clutter.
Great point about the drawing! I've dimensioned everything on the drawings using the smart dimension tool, so changing them doesn't change the part. I did this because if I used the dimensions from the sketches it was one big mess. When I redesign everything I'm going to take that into account when dimensioning everything, including the place where I put the dimensions.
Arno Goossens wrote:
Great point about the drawing! I've dimensioned everything on the drawings using the smart dimension tool, so changing them doesn't change the part. I did this because if I used the dimensions from the sketches it was one big mess. When I redesign everything I'm going to take that into account when dimensioning everything, including the place where I put the dimensions.
You will save yourself a lot of work when you learn to use Insert Model Items on your drawings. Do your sketches well and clean and then the drawing is so much faster.
SWX is not Inventor and Inventor is not SWX. Don't expect them to be. If you can create good models and assemblies in one then all you need to do is to learn the other system's way of doing things. DO expect them to be different. I have asked SWX for a "system translator", i.e., a Design Table in SWX is the equivalent of a Family Table in Pro\E (Creo), but they have not done that. I think it would help a person find out how to do something in SWX that they already know how to do in another 3D system.
My point is this: you might have very high skill in Inventor, but are experiencing some frustration with SWX. Actually, that is all the more reason to go through the tutorials. You should be able to fly through them since you are not having to learn how to do basic modeling. But going through them will dramatically shorten your learning curve on how to do things in SWX. Trust me on this.
Please do post your file, but also invest in yourself and go through the tutorials. You will be amazed at how much it improves your skill with SWX.
Okay, here is what I found and these are things you should embrace in order to improve your modeling skills:
1. Pulley_Small: First feature has two circles in the sketch, but only one is used for the feature. Cut-Revolve1 has underdefined sketch elements - THIS IS VERY BAD! Make the angled sides symmetric about a center line emanating from the midpoint of the root line segment and they will be properly constrained. This whole part could have been more easily made in one feature, a Revolved Boss that correctly defines the profile such as this.
Note in the image above the centerline of the left groove is coincident with the origin. This conveniently puts an already existing principal plane in the center of this groove, which makes later construction of the belt very easy by selecting this plane. Also note that the right hand groove uses parallel, collinear and equal length sketch constraints. This is so that you only have to make changes to one groove and it will be reflected in the other. Duplicating dimensions is just a recipe for disaster since there are multiple dims that have to be updated and this is often easily missed.
The large pulley has similar problems.
2. On both pulleys it is good to put a sketch on a plane through the center of one of the grooves that only has a circle. This circle should be the pitch diameter of the pulley. Label it as such for later use in making the belt.
3. Your assembly model is floating in space. Fix or otherwise fully constrain something like the box bottom. Just grabbing and moving anything in your assembly messed everything up. This is easily avoided if the assembly is anchored and everything is properly constrained.
4. In reality belts are fixed length, therefore it is a better practice to make the belt part definition a driving length. Leave both pulleys free to rotate and give one of the pulleys a freedom to change its center distance, perhaps constrain the axis of the small pulley to move in an adjusting slot. When you use the fixed length for the belt SWX will automatically move the pulley where it needs to go to satisfy all the parameters.
Normally I would not put this much time into a student project such as yours, but you indicated you have experience with another CAD system so I felt it important to try to help you improve your path in 3D modeling in general and SWX in particular. You are a student and just learning, but that is why it is so important to heed this advice now and make good habits from the start:
ALWAYS make your sketches fully defined.
Make your models efficiently with few features.
Make good use of sketch constraints such as mentioned above.
NAME YOUR FEATURES ON CREATION - this is especially important if your model will have a lot of features, but even more important if someone else will be using your model and needs to understand/change it.
Please accept my comments as helpful and constructive input. I am only trying to shorten your learning curve to prevent frustrations with your modeling.
Also, you really would benefit from carefully going through the tutorials.