Assembling according to a coordinate system 1

[mloew]

There is an old thread on this topic that is out of date: Assembling according to a coordinate sys (thread559-117970). I am using SolidWorks 2007 and want to accomplish the same thing: assemble a component using two coordinate systems. Can this easily be done? The only alternative I see is to create a local system of mutually orthogonal planes on the reference system and use standard mates. Using coordinate systems is far more elegant as there is only one datum feature with all the information needed.

Thanks in advance.

Best regards,

Matthew Ian Loew

http://www.daxcon.com

 

[drawoh]

mloew,

Why does it have to be coordinate systems? Why can you not assemble to faces and planes instead?

JHG

 

[mloew]

It is much simpler to have a single feature (the coordinate system) be used for assembly reference rather than three planes that must be mutually orthogonal. It would be better still if coordinate systems could be defined with offsets and rotations from a reference coordinate system.

Best regards,

Matthew Ian Loew

http://www.daxcon.com

 

[ctopher]

IMO, the coordinate system is easier in the 2D world but not the 3D world.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[mloew]

I don't want to start a riot, but working with coordinate systems is very good in Pro/ENGINEER. I am trying to duplicate some of the advanced techniques I was using with that system on a new project using SolidWorks.

Best regards,

Matthew Ian Loew

http://www.daxcon.com

 

[ctopher]

There are others that know both systems and may know a work around.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[TheTick]

Welcome to my world, Matt.

 

[Bester2]

mloew,

I agree and understand your question and thought that doing this was a given. I seem to remember when I was working in Pro-E you could do a coordinate system mate that fully defined the position. If I am not mistaken you could also define the offset from the x, y, and z axis. But I just for the first time tried to do this in Solidworks 2007 and could not do it. I was working in Pro-E on a vehicle project where hard points were used to define suspension points that were later run in an ADAMS simulation. It helped when adding suspension components. All you had to do was model that part with the hard point at the 0,0,0 point then use the coordinate system mate to place in in it's correct place. If I am correct and this can not be done then an enhancement request would be needed. If I am wrong please someone tell me how to do it.


Brian
SW 2007 SP 5.0

 

[mloew]

Brian,

Thanks for the reply. You have confirmed the limitation, unfortunately. I've never submitted an enhancement request, any recommendations?

Best regards,

Matthew Ian Loew

http://www.daxcon.com

 

[Bester2]

mloew,

I just submitted my first enhancement request. Who knows if it will help but I am absolutely shocked that SW can not do this. I always assumed that this was a given. At my last company we were not allowed to reference any feature that was not an assembly datum feature. The easiest was to do this was mate the part to the features to get it in the correct place, then break all of the mate, then use the coordinate system mate as a catch all. That way you would have no failures when you removed parts from an assembly. It also helped by cutting down on the number of mates in the top level. If you are modeling a huge assembly this is one of the best way's to go (skeletons also work but take a lot of forethought).



Brian
SW 2007 SP 5.0

 

[mloew]

Brian,

Absolutely! It is very good practice to not have references to component features. Capture the design intent with skeleton geometry and build your assembly from there. I was stunned to not be able to do this with coordinate systems in SolidWorks.

Best regards,

Matthew Ian Loew

http://www.daxcon.com

 

[MadMango]

I use sketches & extra planes as "skeletons" a lot, and end up with "only one datum feature with all the information needed." I create a part file that contains these sketches and planes, and insert that into an assembly as my skeleton. All other parts are created in-context.

I'm sure many here share your pains with SW, and just as many will be eager to lead you into the light.


"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[madvlad]

I would also like to be able to use coordinate systems, because when some joker makes a part which I have to put into my assembly...somewhere...I dont know where it goes. Instead, he just puts a CSYS in the file to help me out. And if he wants to move his part, he moves the CSYS inside his file, instead of relying on me to keep up with him.

I generally drop things at 0,0,0 and fix them there, and do things in context from a skeleton part (fixed at 0,0,0) like MadMango.

Funny glitch I found (first!): Supposedly when you insert a component... and hit the green checkmark button, it puts it at the origin. Try it... Make a new assy, and put a part at the origin. No big deal.

Now, make a camera, unlock it, set the view to look through that camera, spin it around and stuff, and then insert another instance of the same component at the origin...and the part goes to some different random place! Camera origin? haha

You gotta wonder how the programmers managed to link the part placement code with camera position. It drops in at the correct location if you have the camera locked, so obviously theres a bug which they half-fixed. but wth?

I'm using SW2k7 SP4.0.

Chris

 

[EdDanzer]

I have never used Pro E but in SolidWorks the origin is 0,0,0. If you design each part from the origin and mate using the origin and one plane this should give the same results.

Ed Danzer

http://www.danzcoinc.com

http://www.dehyds.com

 

[mloew]

Ed,

While your solution will work, it fails to capture design intent. Imagine as an example the tires on a car. There is no relation in the context of the tire to the vehicle origin. I'm going to want to assemble the tires to a reference on the suspension (skeleton).

Best regards,

Matthew Ian Loew

http://www.daxcon.com

 

[EEnd]

I remember a more recent discussion on this topic, but failed to find the right key words to make it pop up in the search. Mating all of the components to a common origin was mentioned as common practice in aerospace and automotive. A name was given to the common origin, but it escapes me. If you could find that thread it may be relevant.

If the coordinate systems that you want to mate happen to be the model origins, you can mate the 3 default planes. It should not be too hard to modify one of the macros posted by handleman in: thread559-175155 or by KenBolen in thread559-179434 to mate all three at once.

If the coordinate systems are not the model origin, then you could create a macro which would create reference geometry at the coordinate system which you could then mate to using something similar to the above.

Smart mates may also be a way to automate the process, particularly if you are creating the reference geometry based on a coordinate system.

Eric

 

[EdDanzer]

When I design equipment that the parts may be reused in another design it is best to define mate geometry on the individual parts to make mating in the feature manager and interchanging parts and subassemblies possible. If an assembly is physically large relative to the fasteners this can speed up assembly. The subassemblies (your suspension) and the wheels with tires can be preassembled then inserted into the main assembly to define wheel base. You can then make the subassemblies flexible in the main assembly to allow doing kinematics. By doing file save as on the tire and wheel parts, the wheel and tire subassembly and using mating geometry you can interchange different tire and wheel combinations without loss of the mates by using the replace button.

Ed Danzer

http://www.danzcoinc.com

http://www.dehyds.com

 

[Bester2]

Ed,

I agree that working with suspension geometry can be accomplished other ways than with coordinate system mates. And I know that I brought up the whole suspension topic. But the original post does not specify that they are working with suspensions (I deduced this from his area being automotive and previously working in that area I knew that coordinate system mates are used when assembling suspensions). But I strongly believe that having the option to use coordinate system mates as in Pro-E would be beneficial to SW. I also know from speaking with some of SW's executive staff many improvements come from user’s request. Therefore submitting multiple enhancement requests for this feature would be beneficial. I could see where this may limit companies from the automotive and aerospace industries from selecting SW as their CAD system. Also this feature on the surface does not seem that hard to add.

OK that is all of my $.02
I will shut up now

Brian
SW 2007 SP 5.0

 

[drawoh]

Mating all of the components to a common origin was mentioned as common practice in aerospace and automotive. A name was given to the common origin, but it escapes me. If you could find that thread it may be relevant.

EEnd,

I have not worked in aviation or automotive, but I have designed complex mechanical systems on a drafting board. Somehow, one must keep track of where all the components are. On a simple design, you can scale off your arrangement drawing.

On complex stuff on a drafting board, it is hard to use round dimension values, and things just get complicated. I defined a zero point, and I located everything using absolute coordinates. I do not recall a term for the origin, but someone refered to my coordinates as "stations". This defintely is done in aviation and marine design.

I have not done any of this with SolidWorks, or even AutoCAD. CAD gives me a precise, scale model. I think this problem and this solution have largely gone away.

JHG

 

[drawoh]

mloew,

Why should mating planes be mutually orthogonal?

Good assembly practise in SolidWorks is to not use any more constraints than you have to. Locating to three planes is a nine-point constraint, as opposed to the six-point constraint you actually need.

On quite a few occasions, I have inserted planes into my parts so that I have a mounting face in a convenient position. Consider o-rings. I want to mount to the front and rear faces, and in o-rings, these are not flat. Tangent faces are not completely predictable. On my o-rings, there is a front and rear plane. You can locate a plane anywhere you want, in any orientation you want.

Would this not accomplish what you are trying to do?

JHG