First off thanks for your continued efforts. My main goal is to able to revolve the shape defined by these 500+ points to be able to manufacture it. When I import these 500+ discrete points, they appear to be connected by straight lines, which is an acceptable form of approximation, it's just that I can't seem to create a revolution with this import? I keep getting the error message that the profile isn't closed, yet upon closer inspection SE appears to have connected these points as illustrated in a few posts above. It's for this reason that I thought of perhaps approximating the points with a curve, but ideally the 500 connected points would be sufficient. Maybe revolving these 500 connected points is easier, but I am just doing something wrong?
tomorrow I'll try a couple of experiments with different curve fitting methods and I think I should be able to give you an acceptable means of doing what you want.
I tried to open your part & draft files on my work PC, but appears you are using an academic version of Solid Edge.....so I was restricted to my kids laptop, with ST7 Student Edition.
I discovered that there are a couple of line breaks in the geometry in your part file. Strange thing though, I was unable to get the IGES file to open at all.
I copied the geometry from your part file, into a new Syncronous sketch, and as soon as I had fixed the line breaks [of which there were three] the it displayed the shaded closed region, so was ready to use for the revole operation.....as seen below. [also attached is a Parasolid file of the model]
Becauses there are soo many facets in the sketch geometry, the model has a very heavy topology, so I have it displaying as a shaded model, as having visible edge lines obscures the external contour.
I will be interested in what Frank comes back with....as I was unable to run my other software on my Surface Pro3, I guess my 12 year old program is not compatible Windows 8.1.
Design Manager Streetscape Ltd
Solid Edge 2020 [MP0] Classic [x3 Seats - Cloud Enabled]
Windows 10 - Quadro P2000
I've had a play with the points files and found the same problems as Sean in that I can't open the IGES file and there are 3 disconnected areas on the Part file.
Using the Part file as input I created 2 solids.
The first is similar to Sean's (except I used Ordered and get a 'sick parent error'). I exported this in Parasolid v9 format and it should load into SEv20. It is however computationally heavy and has a file size of 3.5Mb. If it is opened it should be viewed with visible edges turned off.
The second model I created I did by simply fitting a spline curve to approximate the points. At present it has around 14 interpolation points and a maximum error of around .3mm however I could reduce this to any value by editing the curve (adding moree points until a desired compliance is obtained). This model behaves well and is only 700Kb in size.
I am about to try fitting a curve with another piece of software and I'll get back if I find anything useful.
Given that you are using an academic version of SE you could, if you have a suitable PC, download and install ST8 if you wanted to. If so I can give you the original curve file above in Part format.
This might be a useful compromise. I created a DXF file from the Draft file and read this into Rhino 5. Next I refitted the curve in Rhino with a0.05mm tolerance. The new curve seems to behave well and was exported as Parasolid file:
The Parasolid file imported into ST7 but you can try it in V20. Then I created a sketch using the Include command and then completed the profile/axis. Next I used the Revolve command to create a reasonably efficient and accurate solid.
Frank and Sean,
Your advice and time has been of the greatest help to me. I've had a few test pieces manufactured today and the result is more than satisfactory. Many thanks!