Building Spline outside of ProE, then Importing 1

[treddie]

Howdie.
Does anyone know of a way to get a text file of coordinates that when imported into PRoE, ProE then INTERPRETS as a spline? I am trying to avoid building CAD files like DWG, DRW, AI, etc, by just importing raw spline coords as text data.

Thank you very much,
treddie

 

[cadcamguy]

lets see, you need a sketcher csys a spline with at least 2 points

right click the spline ...modify then the file options will come up

points need to be in a .pts file format something like;

0 0 0
0.002408 -0.007695 0
0.009607 -0.015563 0
0.02153 -0.022735 0
0.03806 -0.028997 0

you want the end point of the pts file to jive with the endpoint of your spline before you import

 

[cadcamguy]

now there is something really cool here.

airfoil shapes ... based on pts from 0 to 1
most files are the bottom and top combined, you want to split it into the bottom and top as far at the pts go.

you draw your spline a line from the sketcher csys out some value.... then modify that to 1 or what ever your pts files endpoint is....import the points... finish out the sketch

now if you modify the 1 value , the spline keeps the orginal ratio and you have the same shape longer or shorter
... you then can export those for new values in a new pts file.. from modify if you edit defination

 

[treddie]

Hi cadcamguy.
Thanks for the quick response.

I think I'm lost.

When I right-click the spline, I do not see "modify". Do you mean "Edit Definition"? If so, there is no file options dialog that comes up.

If I am in Sketcher (Intent Manager active), left-click the spline to select it, then right-click > select "Modify" I get the standard spline modify bar down on the left of the screen, but no way to import a .pts file.

If I am in Sketcher (Intent Manager off), the situation is similar.

If I'm in Legacy, right-clicking the spline in the feature list DOES bring up "Modify", but no file dialog appears.

If I then go to Insert > Shared Data, I can import the points, but thewn ProE expects me to build facets.

I am using W3(M030).

Totally lost,
treddie

 

[cadcamguy]

If I am in Sketcher (Intent Manager active), left-click the spline to select it, then right-click > select "Modify" I get the standard spline modify bar down on the left of the screen, but no way to import a .pts file.

can't say for 3 being on 2....but you should have a change in the top left of your screen that wants you to pick a sketcher csys...

 

[cadcamguy]

tryed to upload image to fileserver...server troubles

once you pick the sketcher csys the read file and save file should become available

 

[cadcamguy]

should be some pulldowns top left corner that are;

Point Fit File

in sketcher>intent mangler on

 

[treddie]

Naw...nothing anywhere asking me for a csys.

I'm assuming I should be in Sketcher. The only thing I see after having built the spline and doub le-clicked on it, are the Point, Fit and File menus at bottom left. If I go into File, The file open/save icons are greyed out, so that's not an option.

treddie

 

[treddie]

Started over. Used Sketcher Tool to build my 3 point spline (start point, interior point and end point). While still in Sketcher, I selected the spline and right-clicked > Modify. That gave me the Point/Fit/File menus on bot left. I clicked File Menu, and got a request for a csys, but ProE won't let me select a csys, and the File Open/Save icons are greyed out.
I'm doing something stupid here.
treddie

 

[treddie]

Hold on. I wasn't using a LOCAL csys. I'm going to go eat and come back later and figure this out. I'll email back later tonight.

treddie

 

[cadcamguy]

yes.. you need a sketcher csys ... normal csys doesn't work

 

[treddie]

IT WORKS!!! IT"S ALIVE!!!!!!!

Thanks for your help there cadcamguy!
Much appreciated,
treddie

 

[treddie]

Now that I know about .pts files, and kind of now what to look for now, I did a web search and discovered another text file format that I have seen in ProE but didn't know anything about...the .ibl format. This enabled me to do essentially the same thing without being restricted to the 2D world of Sketcher. cadcamguy > you probably already know about it, but for those who are new to it like myself, the info can be found at:

http://www.proe.com/connectqna_submitanswer.php?cpfeatureid=7581

But here is my procedure taken from that information:


This procedure uses the Imported Blend File (ibl), text file format, and is built in NotePad.

Simply create a header for the file:
Open Arclength

Immediately following the header, go the point coords for the first curve in xyz format:
Begin section ! 1
Begin curve ! 0
3.473 6.125 9.912
2.107 3.673 7.385
7.776 21.782 11.987
3.009 1.6707 3.312

Immediately following the last data, go the point coords for the next curve in xyz format:
Begin section ! 2
Begin curve ! 1
7.475 2.178 7.219
6.734 6.444 1.922
10.212 -3.326 -1.333

...And so on, for as many curves as you need.

NOTE: The website I got this from did not repeat the "Begin section ! x" line for each curve points set as I show it above, but it didn't work when I wrote the file that way. AND DON'T FORGET THE INCREMENTING OF VALUES FOR EACH "Begin..." line.

Once the file has been created, be sure to change the .txt file extension to .ibl.
----------------------------------------
In ProE select menu Insert > Model Datum > Curve.
Select Menu Manager > CRV Options > From File > Done, then:
-Select desired CSys.
-File dialog will appear. Select file type - .ibl, and select the desired .ibl file.
The datum curves should appear.
With regards to building surfaces:
Next, choose to "Insert Boundary Blend", select the curves you want to skin from and to, and you will see your surfaces begin to appear (note the command for this in Pro/E 2001 and prior is "Feature > Create > Surface > New > Advanced > Boundaries").

If a change is required to the coordinate points, simply "Edit Definition" of the curve file and cut and paste the new XYZ data. You will see you surfaces update based on the new data.

 

[cadcamguy]

treddie,

ibl's pretty powerful too. You can get iges info over and then edit is as ibl... if you create curve from file and use iges.. when you go > edit definition >curves... edit..you get the ibl file format ... and it writes that file to your work dir...

so here's something else you can do with the spline pts file.

if you create it as a sketch.. a .sec file..save the .sec

then in part mode make a traj.,and do a vss.... when you go to the vss sketch,

draw angled construction line.. set the angle to some value without 15 decimal places ..then sketch>data from file>pick your .sec .... set the angle the same as const. line... change drag point to the import csys.... place

then mod the angle just to make sure it aligned to the line
now you can make it helical..or have different sizes at each end of your trag... ...make some pretty wild shapes.

 

[treddie]

Too cool...too cool. Lots to experiment with.
Thanks for all the help.
treddie

 

[cadcamguy]

no problem treddie..have fun