a sheet metal part from another inventor part
So that part comes in from our company as a step file. In my mind i am merely trying to use the part to define size of the new sheet metal part and hole locations. The new sheet metal part would be a hat bracket underneath the posted part. Below is from AutoCAD and how i created two views. I am trying to learn inventor, and this scenario is done a lot in our group.
Yes, keep at it, but trust me... the help you will get from the experts in this forum will be invaluable. As @JDMather suggested, give it a try and them post the results. Yes, you will probably get criticism,... but it will not be making fun of you, rather it will be aimed at helping you learn and improve. We're all in this together, and we all started right where you are today.
BTW... Welcome to the Community! I'm Chris, the Community Manager for Product Design & Manufacturing, and I've learned so much from the people in this community! Let me share some good resources for you as a new forums user. And for more learning, or maybe some fun... take a look at our D&M Resources page too, and make good use of the Shop Talk forum. Let me know if there is anything I can help you with!
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Hello @jpschaef,
This was definitely a solid try, seriously!! Trying to step into the Inventor world having never used it can be a bit intimidating, especially trying to dive right into sheet metal!
So, I looked at your model and simplified it. There's a lot of features that can be consolidated into just a few features that I'll try to step you through...also, I apologize now, but I should have created a screen cast to show how I worked through this, but it's a bit late and I definitely wanted to dive in and try to help right away.
The first thing that I do when creating a sheet metal part is figure out how I can quickly model the flanges. 9 times out of 10 I'll create a contour flange where I get all of the dimensional information from a PDF, DXF, STEP File, etc much like you did to get the information you needed to create the model.
For the contour flange, I created a new sketch, and created a profile that would mimic how the part looks if you did a section view. To help make everything symmetric, I projected the YZ and XZ planes, and drew what you see below:
Once I completed my fully constrained sketch, I selected the contour flange option:
Within this option, you can specify which direction you want your part thickness, your bend radius, and which direction you want to extrude. Play around with the feature in my model to see how this changes the part.
Next, I created a sketch and placed all of my holes. I projected pretty much the entire part (that's just because I get a bit lazy...Shhh, don't tell my boss), as well as the XY and YZ planes. Since the holes on one side of the part is a mirror of the other side, I laid out one side, and mirrored the others...helps saves time instead of trying to individually trying to dimension each hole. Once all of the holes are fully constrained, I finished the sketch and applied a Cut feature that goes through the entire part:
I pretty much applied the same logic for the holes on the sides. However, you'll notice that I only dimensioned two holes in the X-Axis and two in the Y-Axis. I then used horizontal and vertical constraints to fully constrain the sketch. I then did a Cut and selected All for the extents.
A little extra:
The A-Side definition helps determine how the flat pattern will unfold. This will also help determine which dimensions will bend up or down in the drawing layout when you apply the Bend Note Feature.
