To place this part in the assembly, take a close look at what really has to be connected...
It is impossible for te faces of the plates to match the faces of the cilinder. What will happen if it's placed right? The edges of the faces will be on the cilindric surface. To accomplish this, use the 'connect' relationship.
After placing two 'connect' relationships, the part is not fully constrained yet, it will move along the cilindric surface, up and down and around. So you will have to put in a 'mate' or 'planar align' to constrain height and position...
Assuming the three plates are a subassembly, you could create a sketch from the top view of a circle that matches the diameter of the tube. The edges of the circle will be connected to the inside edges of the vertical plates. Return to the main assembly and use an axial align between the circle (show sketches in the plate subassembly) in the sketch and the axial centerline of the tube.
This type of connection is REALLY easy with Inventor and Solidworks... Why are these types of mates this convoluted in Solid Edge? Why is SE primary design industry?
I am charged with evaluating some different MCad softwares for my employer, he is leaning to solid edge, but everything about it seems more complicated that its less expensive competitors; where does this product shine?
I'm not as familiar with how the constraints are performed with Inventor or SWX. How is this type of constraint created in each? No matter what package you use, you still have to get the plates on the surface, constrain it up and down and then around the circumference of the cylinder.
As far as the strenghts in SE:
You can create sketches first and then use them when creating features or you can create a sketch during the feature creation process. This gives you a lot of flexibility.
Solid Edge has very strong sheet metal creation tools. This is why I purchased it several years ago. The ability to make flat patterns and pull them into drawings allows me to use them to create prototypes in house.
You can use SE's Direct Edit tools to make changes without having to go back into the history tree and remember how you created the model days, weeks, months or years ago. This can also be used to track changes you've made to the model. Direct Edit is also extremely valuable for editing "dumb models" imported from other packages.
Solid Edge has used the workflow that is now being emulated by other packages.
Draw in view. When you have created a drawing from a model, you can go into the view and add lines etc. I use this tool to draw in wire routing etc. Solid Edge does have a wire harness tool, but I don't have it. I find this tool very useful.
I'll try to think of more. Selecting a package really depends on what you do and what features you find most valuable. Although I'm partial to Solid Edge, the best plan is to test drive each package and make the sales people show you how to use the software to perform the tasks you need. Don't let them drive the demo - put them on the spot and make them show you what you want to know. See if you can get a 30 day trial for each package.
The connect relationship only works for points, lines or planar elements. (in V19 - not sure about V20).
I agree it ought to be possible to connect a point etc to a curved surface.
In this case, to constrain the side plates to the cylinder you can use a Parallel relationship between the inside edge of one (or both) plate(s) and the cylinder, defining the offset distance equal to the radius of the cylinder.
Then add align/mate/angular relationships to fix the rotation and height positions of the bracket on the cylinder.
Just out of interest, how would it be done in SolidWorks and Inventor? - do they allow connects between linear and curved elements?
arlenn
Choosing an MCAD package is all about the main focus of your business. All have strengths and weakness. We evaluated SW, IV and SE, getting the VARs to model our sheet metal product. IV's capabilities were basic and simply did not have the tool set to model the product - the VAR left unable to model the product(i note the latest release has added sheetmetal capabilities). SW could do it but was slow and relied on the feature library for many items. SE was by far the fastest and had an excellent set of dedicated sheetmetal tools.
So for us, SE had the strength in our business focus and we could live with the shortcomings in other areas.
1. Sheetmetal (Even NX is adopting some of the sheetmetal functions of SE)
2. The handling of big assemblies (For example the new zone function in V20 is really good)
3. You can have open sketch profiles in part features.
4. The simple Smartstep bar to guide you through a command.
5. Stable, V20 that is. (Rumor has it that SW 2008 is not so stable)
6. Some new features of SW 2009 have been in SE for quite a while now (For example automatic lip creation and designs Sensors).
7. UGS (Siemens PLM now) owns Parasolid, the 3D kernel used by SE and SW. Dassault have acquired ACIS which put Inventor now in a spot of bother.
Hi Arlenn,
I used SW for 6 months a couple of years ago but don't remember exactly what each constraint type can do.
As I said, some of the constraints could do with improving a bit but SE does recognise axes, points and lines, it's just that they are not always relevant to the type of constraint being placed.
I found assembly in SW to be rather messy, especially when you had quite a lot of parts in the model - it was much more difficult to get the correct faces.
In SE you can set 'reduced steps' on or off to make location of the correct part/face easier. It's nice to be able to say 'this is the part to constrain, this is the face, this is the part to constrain to and this is the face to constrain to'.
I also found it annoying that I could not lock an axial constraint with a simple one-click as you can in SE - you had to add another constraint to fix the rotation.
The 'Capture Fit' is, in my opinion, one of the most useful commands in assembly. To be able to save the constraints to the part file, OR just save them for the current session, is something I use a lot.
If only we could take the best bits of all the systems !
Schipperus - I know it will not give you all the wire harness details, but you can use the FRAMES functionality to create cylindrical sections to represent your wire paths, or pipes/tubes if you don't have XPressRoute. You will need to create some wire models with the correct sections.
It works almost identically to XPressRoute.
Hi Arlenn,
Just reading your last posting again where you say about SW and Inventor -
"They also have Axis and point elements, not just planes, which are also nice, an axis can be mated to axis."
Don't forget that in Edge you CAN locate keypoints, edges, faces, planes, sketch elements, and axis of revolution of parts when positioning.
You do not need to create an axis for the centre of a cylindrical protrusion/hole/cut - that is always implied - so to axial align two cylindrical faces it's just a matter of picking the command then picking one face then the other.
Similarly the centre point of a circular edge is locatable as a keypoint, as are end and mid-points of edges.
