Creating cut out in sheet metal

peter_paton

Hi,

I'm trying to understand from a very basic level how to create a cut out in a sheet metal face.  The rear panel has a through hole which I managed fairly easily but the front panel has a half hole cut into the bottom of the panel .  I have tried to both a) form a hole and b) draw an arc and extrude but without success (extrude 3 will show what I am trying to achieve) - the link is https://cad.onshape.com/documents/476aeb9f08a4edb8bec830b2/w/b6f65d4760b3886eae9751d5/e/bd442b9ff75c3798a6b4e501 if anyone can assist.  Thanks in advance!

john_mcclary

You don't have any bend edges selected, so I can't tell if you intend to  bend on this edge or not.

Because you created all of the sheet metal plates, it still treats this as a single part sometimes.
So creating the half moon cut out right on the edge was causing an error.
If you extend the cut out straight down (as shown) then it will work.

if you really don't want this, then I would have not used sheet-metal, Instead use extrude or thicken unless you plan on bending edges.



Here is another way to trick the sheet-metal tool.

Create your contours before the sheet metal feature, then clean it up

doing it the other way seems to leave these artifacts behind that replace face won't fix either, So I'd do the pre-cut shape, then convert/thicken to sheet-metal afterwards. That seems to be the best solution for me most of the time anyway.

peter_paton

Thanks John, the cut out arc will be on the lower edge without any bend.  The idea was to provide a cutting list for the panels required which would be seam welded in real life. I have done this the old fashioned way - by hand - but thought it would be a good exercise to practice in Onshape, but as usual it proves to be a bit more frustrating than expected! I tried doing it with extrude but ran into difficulty with the feature(s) appearing on both the front and rear panels which is not correct. After watching one of the tutorials on sheet metal it seemed logical to use that feature since this is in reality a sheet metal construction. 

john_mcclary

I see.

So you only need sheet-metal feature if you want a flat pattern of a formed part.
Otherwise you are just adding work. Sheet-metal has a lot of rules associated with it.

It would be better on import the parts into an assembly to create your cut-list.
Or use a feature script to push dimensions into your part properties then use a custom table to see your stock list. 
This method won't care about what method you used to model it. (unless you want a flat pattern dimension, that part would need to be  made with sheet-metal, for example: your top curved part)

https://cad.onshape.com/help/Content/custom_tables.htm?cshid=custom_tables

john_mcclary

Here is "part bounds" table for example; but it doesn't account for sheet-metal (they should all be the same thickness..)

matthew_stacy

@peter_paton ,

OS sheet metal tools have a few idiosyncrasies, as well as unique capabilities, that I have only begun to embrace.  One issue is that for whatever reason, you can't cut-extrude thru the sheet metal (at this particular location), as you are trying to do with Extrude 3.  I suspect the concern is how that cut might interact with a bend (if you were to subsequently edit the Sheet-Metal-1 feature to specify a bend along that bottom edge).  Potentially messy.

You CAN however insert a Finish-Sheet-Metal feature BEFORE Extrude-3.  The downside is that this cut will not be included in the flat-pattern.

But here's the good news.  You can sketch and Extrude-Remove, directly on the sheet metal pattern.  You don't even have to specify and end condition or depth.  It will cut thru the sheet period, no questions asked.

So often when I'm struggling to accomplish a seemingly simple task in Onshape, I discover that I need to escape from familiar workflows that I developed in SolidWorks (insert your prior CAD platform of choice).  I often flash back the the warden's advice the movie Cool Hand Luke, "... got to get your mind right Luke." 

Cheers,

Matt

(struggling to get my mind right)

peter_paton

Thanks Matt, my problem is that my previous drawing experience is limited to pencil and paper (which I ended up doing for this!) but I am somewhat keen to learn at least some basic CAD using Onshape.  I have managed to get a bit further (a couple of unscheduled days off work has given me a bit time to delve in again) but stuck again as this part does not have a floor and I cant see how to delete that face on its own so appreciate any guidance on this too.  Link  https://cad.onshape.com/documents/04e73a6536338cbc2e9f4568/w/2c5f55ebb1a09504ed793195/e/a56e1f0007f3aa704d7c47dd

Cheers,

Peter

john_mcclary

Oh, if you don't need the bottom part then all you need to do is edit the sheetmetal feature, unselect the bottom face (if you used thicken)
Or add the bottom face to the list of faces to ignore (if you used convert) 

Then there would be nothing in your way to cut that bottom arc, and the original problem would have never been an error 

peter_paton

Hi John, after your earlier advice and watching a few tutorials I did this one by extrudung the basic shape and using the shell function. So far my efforts to select and delete the floor face have resulted in deleting the whole item. I'll have another look at the animation you sent last time, i may find the answer in there.  Thaks for your time and help.

peter_paton

PS - I had a brainwave - suddenly thought maybe if I select the floor and use extrude - remove I might get a result.  Worked perfectly!

john_mcclary

You can exclude the face with the shell command directly also.
No need for additional features

peter_paton

Thanks John, once again extremely helpful.