I have a lofted sheet metal part and need to create cut-extrude.SW don't recognize the flange face as as a sketch plane.
Pardon the delay, weekend you know.
I simply edited the flange sketches.
A Flange Profile Sketch (highlighted in blue here) can be edited like any other feature sketch after you have made the flange by RMB it in the Feature Tree and selecting Edit Sketch from the pop-up menu.
The sketch will open for editing and can be modified like any feature sketch.
You can also edit the Flange Profile Sketch while you are creating the Edge Flange by clicking on the "Edit Flange Profile" button.
Note that in the dialog box that pops up in this case clicking the back button does not undo your modifications to the sketch profile. It just takes you back to the Edge Flange Feature Manager so you can change other variables, or if you are making more than one flange you can select and edit their profile sketches before you finish the feature.
If you are making more than one flange in a single Edge Flange feature, select the edge for the flange you want to modify and then click "Edit Flange Profile".
If you are making more than one flange it is possible to give them entirely different shapes. However the bend angle, radius, flange position, relief etc. are the same for all flanges in a single feature. The flange profile sketches are highlighted red here.
A few thigs to note.
Flange Profile Sketches have relevant horizontal and vertical relations by default some of which you may need to delete. Don't delete the on-edge relationship. The flange length is not initially determined by the sketch (note the blue underdefined line) but if you can add a dimension or relations if desired, if you do, note that the option to set the flange length in the FM will be greyed out.
Another way to make the flanges at an angle would be to make them oversized (if your design allows) and then add a cut or two, something like the image below (which is of the attached file so you can have a better look). You could cut each flange to shape separately if that were more applicable to a particular situation.
Each of these methods (and there are certainly more) has pros and cons depending on the particular situation, so which to use is up to you.
Generaly speaking a loft, even if it looks like it should be planar, will be problematic to use as a sketch plane.
I'm assuming the part in question is the U shaped one. From your screen shot I can't see any reason that it shouldn't be made as a simple U shaped Base Flange. That should give you no problems using the surface as a sketch plane.
Eric, Thanks for the reply.
I tried a Base Flange ,but didn't work since i have various angles and tapers.I tried creating solid bodies ,then Convert to sheetmetal with unsatisfactory results.
Have you tried to create the sketch on a plane then doing your cut up to the back surface?
Can you post your part? It doesn't look like it should be that hard to make.
Still on SW 2010 here, getting ready to make the jump straight to '12 but not quite yet. If you are '11 or higher can you post a parasolid?
I'm new to forums,how do I post drawings
In the upper right corner of the reply dialog box is "Use advanced editor"
I'm relatively new to SW forums,how do i post a part?
When making the reply, click the Use advanced editor link in the top RH corner of the Reply box, and the full options will become available. The Attach Files option will be in the lower LH corner.
Here's the trouble maker
Here's a quick and dirty example of how to make a part like that in sheet metal. Something like this will be much easier to work with down the road when you want an accurate flat pattern and need to add more features.
How did you get the edge flanges to angle upward?
Good morning Daniel,
With a last name Blank, you must be close by, did the above work for you?
Insert plane on three of the corner points of the loft and use it.
Thanks for all the help guys!
I wish you'all A Merry Christmas!
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