Hello,
I have been asked to flatten this piece to send out to have die cut for a template. I have noe experince in Sheet Metal work at all. The piece will not be made out of sheet metal. I have used Pro-E for over eighteen years and switched companies a year and a half ago that uses SolidWorks. Can somebody please help me out with this. I have read the help and have had no luck in flattening this. Thanks in advance.
It sounds kind of silly to ask, but did you try the flatten function? (visually in the picture, select red then green box)
(Its a future version so its grayed out for me, but should be active for you)
In the case that the part is not a sheetmetal part already, you can use the "Convert to Sheetmetal" function, and select a face on the part. Just make sure that you enter the original thickness in the 'property manager' when it becomes an option. And once its converted, then flatten it.
Either way, I cant think of anyways to flatten a part if its not sheetmetal, but maybe some of the Surface guys on this forum could help.
1. Insert Bends, picka a usable edge.
Then it becomes sheet metal
2. Flatten.
See image.
Thomas, it took a little bit of trickyness to get your part converted to sheet metal. For the most part, SolidWorks users start a part using the sheet metal tools instead of making a solid and converting it to sheet metal. The sheet metal modelling tools are geared towards preserving uniform thickness and making the cuts normal and adding reliefs and stuff like that.
Now, SolidWorks can convert a solid to sheet metal, you just have to make sure that the solid is uniformly thick and that all of the cuts are normal to the sheet metal faces that they are cutting.
When you did your die cut the direction of all of the cut surfaces was along the z-axis. So SolidWorks kind of balked
I went ahead and added an Insert Bends feature to your part, using one of the edges as the stationary entity ( you have to pick an edge if you want to turn a cylindrical or conic solid into sheet metal). Solidworks ran into trouble flattening the part because the faces produced by your die cut were all parallel to the z axis instead of being perpendicular to the cylindrical surface but I was able to trick Solidworks into repairing the rogue faces by putting unfold and refold steps in there.
I was then able to turn on the display of the flat pattern.
I suggest you read the online help on Insert Bends and Rip Bends which are useful for converting existing solids to sheet metal. (These are not to be confused with the Base Flange which creates a sheet metal body from a sketch and Convert to Sheetmetal tools which allows you to wrap sheet metal around a solid body)
I uploaded a model for you to look at.
See where that gets you.
John,
Thank you so much for the part. That is exactly what I was looking for. Like I said I have no experience with Sheet Metal in my Pro-E days or now with SolidWorks. The model was created by a so called Engineer. The modeling and drawing practices here are not very desirable. I learned a lot by your model. I stepped through your process. Thank you so much.
You are very welcome.
Thomas, it took a little bit of trickyness to get your part converted to sheet metal. For the most part, SolidWorks users start a part using the sheet metal tools instead of making a solid and converting it to sheet metal. The sheet metal modelling tools are geared towards preserving uniform thickness and making the cuts normal and adding reliefs and stuff like that.
Now, SolidWorks can convert a solid to sheet metal, you just have to make sure that the solid is uniformly thick and that all of the cuts are normal to the sheet metal faces that they are cutting.
When you did your die cut the direction of all of the cut surfaces was along the z-axis. So SolidWorks kind of balked
I went ahead and added an Insert Bends feature to your part, using one of the edges as the stationary entity ( you have to pick an edge if you want to turn a cylindrical or conic solid into sheet metal). Solidworks ran into trouble flattening the part because the faces produced by your die cut were all parallel to the z axis instead of being perpendicular to the cylindrical surface but I was able to trick Solidworks into repairing the rogue faces by putting unfold and refold steps in there.
I was then able to turn on the display of the flat pattern.
I suggest you read the online help on Insert Bends and Rip Bends which are useful for converting existing solids to sheet metal. (These are not to be confused with the Base Flange which creates a sheet metal body from a sketch and Convert to Sheetmetal tools which allows you to wrap sheet metal around a solid body)
I uploaded a model for you to look at.
See where that gets you.