[Smitty092000]

My name is Mike and I have been teaching myself Solidworks using the 2009 SP 3 seat that we have in the shop i work in. I'm not doing to bad at it but i'm starting to have a little trouble getting my round tube parts to mate correctly. Im building a tubular type frame assembly out of 1" diameter aluminum tubing. Some of my tubes have square cuts on the ends and some are coped and mitered to fit together tightly at their respective junctions. There isnt anything to fancy regarding the design, all junctions are 90 deg joints.

My question is this: Are there any handy tips or tricks to getting my coped pieces to fit to the other tubing easily? Some of my tubing parts are mitered so that more that one tube fit together at the same point around a common tube if that makes sense. I can mate my tubes together by their miter but I cant get that assembly to mate correctly around the tube they share.

Thanks in advance for any help you may be able to give and I apologize for not being able to provide examples at the moment but their are just too many restrictions on government computers.

Mike

[small_toys]

Are you using weldments? I think this would help alot if you are not.

[Smitty092000]

I am not using weldments. Not exactly sure what you are refering to really or how they work. Sorry for my lack of knowledge but what little bit I do know of this software is all self taught.

If you wouldnt mind a quick dirty rundown I am more than willing to give that a try and see if it fixes my problem. Thanks for the suggestion though.

Mike

[JerryFlyGuy]

W/out a doubt weldments would be alot faster. Imagine using sketched lines to define the size and shape of your complete model. Then going through the model and selecting various lines and applying a material [tubing] to each line. The miters and copes take care of themselves. Very quickly you can create a weldment frame of pretty much anything.

It is certainly something to look into learning, however it is concidered a more 'advanced' modeling method. [Not were a person should start learning Solidworks]

As to your current question. I typically use planes and points for something like this. Makes sure there are planes through the length of the part [down the axle length and perpendicular to the length etc] as well as points on the ends of the pipe and using these you can make most of the needed mates. It does depend to some degree on how complex your model it [ie if your designing a car frame or a bike frame [hard] or a broom rack [possibly easier]]

Fwiw
JFG

[cro-magnum]

Youtube offers many tutorials on weldments. I use youtube to refresh my memory on things I have not used in a while. Search Solidworks weldments and also Planes but not at the same time. As Jerry stated planes w/2D sketches will be the easiest way to make your product.

This is how I would build your part. Jerry may have a different method that I would like to hear about.

1. Draw the right side of your frame in right plane (just lines your structural member will follow the lines)
2. Draw the front side of the frame on the front plane
3. Add a plane using the right plane and the sketch drawn in the front plane, you'll probably have to play a little to achieve what you want. In the end you need a plane that runs parrallel to your right plane at the same distance of the width of your frame. Use relations or derive the sketch to build the other side of the frame. That way changes made in the original sketch will change the opposite side.
4. The last plane is easy because you connect the dots and auto relations take over.
5. Find your structural members feature in weldments and select some tubing that will work for you, then just click on your lines.

With that and some youtube you should be fine

Travis

[JerryFlyGuy]

Well, if there is one way.. there are many

My experiance has lead me to build the model as I want to build the part/weldment on the shop floor.

Typically I'll start w/ the base features [alot of what I design is on a skid or base frame of some sort. So I start there. I'm not concerned w/ what goes on it at this point [unless there is needed structure at specific locations etc]

Once I have the base features sketched and then the weldment parts put in I start adding sketchs and details from there. Rarely would I do all my sketch's from the start and then try and put in the weldment profiles. I find that sketching ontop of the weldment faces and profiles [building ontop of existing geometry] to be faster, less buggy and easier to be made parametric.

But thats just the way I do it.. [not saying it's the best or only way ]

JFG

[Smitty092000]

That is the way I try to build my assemblies as well. As if I were physically in the shop putting the part together. I built each tube to the length and specs they needed as individual parts and then I imported all of my tubes into one assembly as if I had them ready to fixture and weld up.

I am considered one of the more advanced people in the shop having taught myself not only Solidworks but Autocad and Mastercam as well. Its easier for me to be able to explain to some of the younger guys how their project is supposed to look and be able to go over what would make their time more constructive if the model I have can represent the parts other people have already cut out.

I do thank everyone for their input and will definately try both the weldment and the multiple plane/point ideas and see what I can come up with.

Mike

[JerryFlyGuy]

Smithy, I think you miss-read me I don't model everything as individual parts. I model in the sequence of the build. In the case of weldments, it doesn't make sense to model tubes by themselves and then assemble them as an assembly.

I model my weldments as a multibody part file. In doing this, I find the coping and cutting of various parts is much more intuative and fast rather than modeling individual parts. When modeling things on their own, part by part, I find that I'm doing way more guessing and math than I need to and this induces human error [now was that a 67deg miter, 32deg off vert or a 32deg miter, 67 deg off vert.. you never have these questions when you do a multi body part file the software figures it out for you]

Fwiw

JFG

[Smitty092000]

Yes I must have misunderstood you. I will definately give the weldments a try. I knew that there must always be an easier way to do something and i just needed a second set of eyes over my shoulder so-to-speak.

Thanks again for all of the advice and I will see if I can post up a copy if I can get the weldments figured out.

Mike

[fatal-exception]

1. Draw the right side of your frame in right plane (just lines your structural member will follow the lines)
2. Draw the front side of the frame on the front plane...

There's really no need to to this. Just use a 3d sketch. Simple as pie.

There are tutorials about 3d sketching and weldments included with SW2009. Take the time to do them and you will catch on quickly.

Paul

[cro-magnum]

There's really no need to to this. Just use a 3d sketch. Simple as pie.

In my lack of weldments experience I have struggled to make prints for a part that is not on an original plane. Now I use planes and 2D to keep it simple. I hole heartedly agree that a 3D sketch is easier, it just causes me problems later.

Travis

[JerryFlyGuy]

While 3D sketchs are pretty niffty and are useful at times. Weldments is not one of the places I used them. Primarily for two reasons. I don't generally do all my sketching in one file [as would be done in a 3D sketch], I prefer to put 2d sketchs on top of geometry and build from there. Secondly a 3D sketch can be a bear to modify later [depending on how complex things get and how drastic the change]. If I sketch in stages and then model the weldment parts in stages I can pull out 'chunks' of the model throw them away and keep going w/out cratering the whole thing [which is very possible when you start rooting around, changing a 3D sketch].

Just my experiance..

JFG

[fatal-exception]

In my lack of weldments experience I have struggled to make prints for a part that is not on an original plane.

Hmmm. I've never had any problems making drawings from them.

...Secondly a 3D sketch can be a bear to modify later [depending on how complex things get and how drastic the change].

I agree with that.

[DMF_TomB]

add reference geometry axis and planes

for cylindrical surfaces have you tried creating an axis. it can be at an intersection of 2 planes or select the outside circumference of a cylindrical surface.

the center line axises of 2 cylinders can be made coincidence or made to touch one another . the plane on a axis of a cylinder can be set parallel on or at a distance from another plane or at a specific angle to another plane.

PS I have read the book Solidworks 2009 Bible and am now reading Solidworks 2010 Bible. I learned much about Solidworks from the Solidworks 2007 Bible.

I suggest learning about all possible mate types and learning about all types of reference geometry

[kelvoden]

My name is Mike and I have been teaching myself Solidworks using the 2009 SP 3 seat that we have in the shop i work in. I'm not doing to bad at it but i'm starting to have a little trouble getting my round tube parts to mate correctly. Im building a tubular type frame assembly out of 1" diameter aluminum tubing. Some of my tubes have square cuts on the ends and some are coped and mitered to fit together tightly at their respective junctions. There isnt anything to fancy regarding the design, all junctions are 90 deg joints.

My question is this: Are there any handy tips or tricks to getting my coped pieces to fit to the other tubing easily? Some of my tubing parts are mitered so that more that one tube fit together at the same point around a common tube if that makes sense. I can mate my tubes together by their miter but I cant get that assembly to mate correctly around the tube they share.

Thanks in advance for any help you may be able to give and I apologize for not being able to provide examples at the moment but their are just too many restrictions on government computers.

Mike

Believe it or not it is very simple to do what you are trying to do and can be done without weldments (that is a whole other way to do it)
Simply make the mate using the planes of the two parts being mated and make a coincident distance mate.

[Smitty092000]

Well I played around a little bit and I got a lot closer than I have before. I still need to teach myself a thing or two so I can get the pieces to trim just the way I want them too but I'm happy with what I have so far. I still have some other components that need to be added to this model such as gussets and things of that nature but I wanted to show everyone what you have helped me to accomplish.

TomB: I have and am reading the Solidworks '09 Bible. I thank that book for nearly everything I know about solidworks. That and the mistakes I've made that actually helped me do something correctly later on.


Thanks again, Mike

PS.. Make sure you rename the attachment from .pdf to .sldprt...

PSS Thanks again

[JerryFlyGuy]

Ahh.. well that surely would have been fun to do w/ anything other than a weldment not impossible but... more 'fun'