OK, I’m sure this is a noob question, but I’m very new to Inventor. Like 3 hours new. I’m pretty good at teaching myself, and have been through some tutorials already.
I’ve made a new file in which I’ve placed a bunch of C-Base chassis channel segments, along with the corner connector things. I’ve got it all constrained together. The thing makes a big square though, of course, since all the chassis bars are the same length. I want to shorten the two horizontal bars so I end up with a “long wheel base” rectangular shape.
I’ve been digging all through everywhere trying to figure out how to isolate one component (or these two bars in this case) and simply change the length of it. I want to make it like 10" shorter or something.
Its quite alright to be new to inventor but the problem you have can be solved albeit slightly mundane.
Open up the parts file for the chassis rail in its normal drawing (not as an assembly)
right click one of the flat, long faces of it (IE, not the end, though it can be done, lets keep it simple =D )
click “start sketch” (or some similar command, it depends on your inventor version)
Draw a simple box over the section you want to cut off, be aware that you keep your spacing as autodesk does EXACTLY what you tell it to, so you might need to cut off 9.5 or 10.5 inches to get the holes lined up properly.
Finish the sketch to enter into the modeling commands.
Click Extrude and select your square, use an appropriate depth to get rid of the bar entirely.
Before you click through on the extrude click the second box under the section where you put in your depth, this should tell it to subtract rather then add. Youll know you did this right if the outline of your box is in red as you look at it from an angle.
Click okay and voila! your C-channel has been cut
go to file, Save as… and save it as a DIFFERENT file, IE C-channel_short_bar *
the name doesnt matter, but it MUST be different or else you just changed the original part and will have to re download it from FIRST or your parts backup.
Instead of cutting it shorter I just right clicked on “extrusion 1” on the left, selected “edit feature”, adjusted the length to what I needed and clicked OK.
Then I deleted hole 1 and hole 2 to clean it up a bit.
This is a better method. If I remember correctly the “C” channels are drawn as sheet metal parts that at folded much as they are in real life. Its a much better practice to simply edit the original extrusion or sheet metal feature, rather than add additional sketches or features to the part.
If you want to maintain an accurate BOM while shortening the rail, I recommend that you add the C-Base Rail to an assembly (presumably called Rail-Short or Rail - Long) and then add an extrusion(s) to cut the rail. You would then make a print of Rail-Short and flag out the use of the C-Base Rail in its construction. Save-As disconnects the new geometry from the old which may not be desirable. Also, if you add information to the AM rail at some point, like a hole or some iProperties (cost data) then none of the Save-As geometry will update, but all the stuff modified at assembly will.
Don’t forget to pay attention to where the holes are in the AM rail are as you shorten it; it may be beneficial to take some material off both ends so that the hole patterns remain centered.
I assume many people use the Kit/Parts files provided by Autodesk or AndyMark (whichever creates them). Everyone should have the same issue then, of having to shorten the C-channel to make anything aside from a square. Again, being a novice, this seems difficult.
I’m getting the hang of constraining things, but I don’t know about trying to modify already-created parts. I wonder if any teams have Inventor files available containing the shortened bars for a “long wheel base” style machine. I’ll look around.
Anyways, thanks to everyone that’s replied so far. Accurate, detailed, and quick answers are why I always come to Chief Delphi first. Thanks!
Do a “Save As” to the modified part, parts with the same name will be the same in your assemblies. You can do a “Replace Part” in the assembly once you have the new file created.
