I am trying to make a sweep pattern of a lip on the I.D. of the fin but inventor is not responding. The RAM usage starts from 5GB and gradually increases to 16 GB in about an hour but does not give me any result. I just close the program after that. Can anyone pleae suggest me how to deal with this type of sweep pattern. Attached is the .ipt file for the part download link. [ "PROFILE TO BE SWEEPED" is to be sweeped along " SWEEP PATH". ] Any suggessions would be highly appreciated.
Can you attach the file here?
Find the red End of Part marker in the browser.
(End of Folded on sheet metal parts EOF)
Drag the red EOP to the top of the browser hiding all features.
Save the file with the EOP in a rolled up state.
Right click on the file name and select Send to Compressed (zipped) Folder.
Attach the resulting *.zip file here.
The CADWhisperer YouTube Channel
I have already tried doing that. The file in its normal state was about 25 MB. Even after moving EOP to the top and zipping it, the file size was more than 5 MB so I had to upload it in Autodesk 360 and share it here.
I tried this only with a small region. It took some time, and it's looking strange. Filesize went up to 254 MB.
IMO, something's already wrong with the startup geometry. 25 MB seems not normal to me.
Walter
Walter Holzwarth
I am just trying to add a curved lip at the I.D. of the spiral along the length of the curve. Is there any way I can make a curved lip that is tangent to the main spiral along the inner edge of the surface.
Nothing seems to be working at this point.
The file is large because it is a really complex surface geometry with multiple curves with spirals that have variable pitch and lots of complex surface trimming.
I am going back the SweepSrf2 - it is taking way too long to create that surface even when I greatly simplified the problem.
The CADWhisperer YouTube Channel
SweepSrf2 is made from the combination of the variable pitch coil projected to the combination of the conical and cylindrical sections of the drum. Since the inside of the coil is trimmed I am having problem to dweep the curved lip. Any suggession to acheive the surface pattern is appreciated.
The root cause of the performance and capacity problems is the Wrap to surface functionality in the Project Curve to Surface command. In Sweep Pattern.ipt, the Project to Surface2 in 3D Sketch6 caused the following problems:
This legacy issue has been resolved in Inventor 2015. See http://help.autodesk.com/view/INVNTOR/2015/ENU/ > What's New > What's New in Autodesk Inventor 2015 > General > General Modeling Improvements > Performance Improvement in Wrap to Surface/Face
To resolve this issue created in Inventor 2014 or earlier, open the part in Inventor 2015, recreate the Project Curve to Surface feature (i.e., delete the old feature and create a new feature), and fix the downstream features.
I used the following procedure to fix the model Sweep Pattern.ipt.
1. Open Sweep Pattern.ipt in Inventor 2015.
2. Move EOP below Work Plane13.
3. Make Coil Curve and ExtrusionSrf2 visible.
4. Press F6 to zoom all.
5. Make Work Plane 13 grounded (i.e., Right-click on Work Plane 13 and select Ground).
6. Double-click 3D Sketch6 to edit the 3D sketch.
7. Delete Project to Surface2.
8. Invoke Project to Surface command.
a. Press Wrap to surface button.
b. Select the cylindrical face in the graphics window.
c. Press the arrow button for Curves in the dialog.
d. Select the Coil Curve in the graphics window.
e. Hit OK.
9. Finish Sketch.
10. Make Coil Curve and ExtrusionSrf2 invisible.
11. Make 3D Sketch6 visible.
12. Right-click on Work Plane13 and select Redefine Feature.
13. Click the new, projected curve and its endpoint.
14. Move EOP below SweepSrf2 (and you will see SweepSrf2 turn red).
15. Double-click SweepSrf2 to edit.
16. Select the new, projected curve as the sweep path.
17. Hit OK.
In Step 17 above, you will see the sweep surface created in less than one second, rather than several minutes! Also, the file size will not bloat.
In Inventor 2015, the curve created by the following command is lightweight and yet more precise.
HTH,
Glenn
Helps with time and filesize, Glenn.
But when trying to sweep, there's still a self-intersection message
Walter
Walter Holzwarth
Glenn, thats a great improvement from 2014 which decreases time and file size. But even after this operation the sweep pattern along the sweep path cannot be made. Is there any new features in 2015 that might possibly help in creating such sweep features?
I was wondering what solidworks would do for the same case. I exported the surface file in .iges forat and did a quick sweep for the same path and pattern in solidworks and it gave me exactly what I was looking for. I have started to wonder if Inventor is inferior in surface modelling in comparasion to solidworks. I am not trying to start a war or anything but why would inventor not do a sweep function that inventor could do in less than a second. I exported the file from Solidworks and opened in inventor and now I am getting "Modeling Uncertainity". Can anyone please tell me if there is any way to get this sweep pattern exclusively using Inventor. The drawing shows the red sweep pattern that is already acheived. The green part is what I am trying to create.