JD Mather Posted October 22, 2012 Share Posted October 22, 2012 Edit Sketch1 Right Mouse Button (here on out RMB) and select Show all Constraints You have a 90° dimension that is not needed. Delete it. Add a Horizontal Constraint the horizontal line. Is the 3.004 really measureable? What is the manufacturing tolerance? Can you make that 3 instead (there are 2 other lines that are 3 in the same feature area, maybe add an = constraint to all 3 so that only one dimension is needed). Quote Link to comment Share on other sites More sharing options...
MKR Posted October 22, 2012 Author Share Posted October 22, 2012 Okay, done, done, and done. Yeah I screwed up last night. The very last thing I did before I saved the drawing was changed up the overall length of the part; I knew it grew to my dimensions, but didn't realize that it created the void you pointed out. Now what? I removed the 90 degree dimension, but why? Does it make a difference not having it vs. having it? I agree on the 3.004", you are talking half a razor blade thickness....on this part that doesn't matter. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 22, 2012 Share Posted October 22, 2012 I removed the 90 degree dimension, but why? Does it make a difference not having it vs. having it? Doesn't really make a difference (in this case) other than a matter of principle for me. I prefer to have geometry constraints rather than dimensions and once you get the hang of Inventor sketching you don't have to add the constraint (Inventor does it for you) while adding a 90° dimension does take effort. My motto is - Get Lazy, let Inventor do the work for you. I'll be back in a little bit (have to go do my paying job). Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 22, 2012 Share Posted October 22, 2012 (edited) ... changed up the overall length of the part; I knew it grew to my dimensions, but didn't realize that it created the void you pointed out. You missed a coincident constraint. That is the beauty of Inventor parametric constraints - when done correctly this constraint should have been automatic and changing dimensions would simply update the part rather than causing it to blow up. Edited October 22, 2012 by JD Mather Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 22, 2012 Share Posted October 22, 2012 I think you know what I am ultimately trying to make here, correct?[/qUOTE] I assume you are trying to derive the four flat pieces of sheet metal Flat pattern from the bent parts that would be required to manufacture this as a weldment? Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 22, 2012 Share Posted October 22, 2012 The previous image of flat was for one of the "sides", this is for what I interpret as the "top". as bent flat before bending. Quote Link to comment Share on other sites More sharing options...
MKR Posted October 22, 2012 Author Share Posted October 22, 2012 YES!!!!! Exactly. That is exactly what I am trying to do. Okay so now what do I need to do to follow you? Question, the sketches that I am drawing are only profiles and do not account for material growth or material needed to actually create the part, do yours? I can follow the side line of the top profile to determine the actual length/ bends of the side and also follow the top line of the side profile to determine actual length/ bends for the top. Is there a way for Inventor to automatically do this for you? The whole point of what I am trying to do is create the 3d part so that I can blow it all apart and have a flat pattern to lasercut. Thank you for what I have learned so far. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 22, 2012 Share Posted October 22, 2012 ....account for material growth or material needed to actually create the ..... Inventor accounts for Bend Allowance (stretching during bending operation). You model to the desired finished dimensions and Inventor calculates what size the flat pattern dimensions should be before bending. I didn't quite understand this, "a square corner seam of .0625" on every edge" as I thought you might just take off the .125 thickness on both sides of the side pieces and have the top and bottom overlap flush to the outside of the side pieces. However you want them to match up is the easy part of the problem though. I'll get back to the problem in a bit. Quote Link to comment Share on other sites More sharing options...
MKR Posted October 22, 2012 Author Share Posted October 22, 2012 Okay, that's perfect. As far as the corners go, I have attached how I wanted all of the corners to be for reference/ clarify. For whatever reason I stated .0625" originally; I would like .125" or .120" since it is 11 gauge to be exact.corner reference.dwg Quote Link to comment Share on other sites More sharing options...
MKR Posted October 23, 2012 Author Share Posted October 23, 2012 So understanding that Inventor accounts for stretching during bending and you supply the finished model; did you draw the inside and bottom or simply move the parts to those locations in your completed drawing above? Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 23, 2012 Share Posted October 23, 2012 I modeled as one part and then derived the individual part that would make up the weldment (Manage tab > Derive Component). Quote Link to comment Share on other sites More sharing options...
MKR Posted October 23, 2012 Author Share Posted October 23, 2012 After the sketch is complete, I assume I need to use the contour roll tool, and then create face? This is where I ended up on the forum... I extruded my part and laid the top profile accross it and split it from there to end up with a whole solid model. I know this isn't correct, but I am lost on how to do it like you did. Do I need to go ahead and recreate the top profile in a second sketch? Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 23, 2012 Share Posted October 23, 2012 Do I need to go ahead and recreate the top profile in a second sketch? Yes, that is what I did. I fudged the top view since I didn't have your dimensions. Quote Link to comment Share on other sites More sharing options...
MKR Posted October 24, 2012 Author Share Posted October 24, 2012 (edited) Alright I have created another sketch (top view; ) it is fully constrained and ready to go. Now what would you do from here? side rail w top rail sketch.ipt Edited October 25, 2012 by MKR Quote Link to comment Share on other sites More sharing options...
MKR Posted October 24, 2012 Author Share Posted October 24, 2012 Hey JD, I need your help still. What do I need to from here? Quote Link to comment Share on other sites More sharing options...
MKR Posted October 25, 2012 Author Share Posted October 25, 2012 I am trying to use the contour flange tool. I went back into the side profile sketch and traced the upper line of it so that I could select it for the flange. I can create any one section with a contour flange, but I haven't been able to do the entire side yet. Any recommendations? I'm not sure if I am using the tool properly or not. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 25, 2012 Share Posted October 25, 2012 There is a trick to doing this part. Do not use sheet metal tools till the end. Extrude intersection Shell Derive Component as surface body (4 times- one for each part) Thicken inside surface (4 times) Convert to sheet metal, set thickness then Flat Pattern. (4 times) Quote Link to comment Share on other sites More sharing options...
MKR Posted October 25, 2012 Author Share Posted October 25, 2012 Thank you so much JD! I have created the part and have shelled it. I still haven't figured out the derive component yet; it wants me to insert a file. I think I can figure out from here. Wow, it was a lot easier than I ever expected to get here. Quote Link to comment Share on other sites More sharing options...
JD Mather Posted October 25, 2012 Share Posted October 25, 2012 Post your master file (the shelled ipt) so that I can check that you did it correctly (that is, the easy way). Quote Link to comment Share on other sites More sharing options...
MKR Posted October 25, 2012 Author Share Posted October 25, 2012 Alright, here ya go. I think I did it correctly....frame profile.ipt Quote Link to comment Share on other sites More sharing options...
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