Sheet metal-part drawing

[maksud.malek]

Hi,

sheet metal parts drawing is very  long and time consuming process  for the simple parts like angle with hole or door  with 4 or 8 bend with fixing hole. Angle and door we have thousands of sizes with  different hole dim.

if I do the  design of the door  with I parts  i can make all size by the typing only but i cannot get drawing  of the that parts within that time. Thanks to supporting software thats software give us DXF within minutes.

Drawing of the first door if we set same we will not get in second  parts when we place it even i don't  to want place it .

i want only parts drawing with bending direction and dim with correct view. Hole and other detail not require because its as per the drawing in DXF . CNC its self accurate to do the parts as per the dxf.  

Anyone can give the idea or advice how to get  fast sheet metal parts drawings  for only to get perfect view with bending dim and direction for the thousands of the door.

[alex.haerens]

You can copy a drawing to a different name. This will give you 2 drawings, referring to the same part file. To get the second drawing refer to another part file you have to "convince" Inventor into changing the model. So you close the #1 file and drawing. Next go into a normal browser window and manually change the #1 part file name (I add a underscore to the filename, anything else will also work). Now you open the copied (#2) drawing. Inventor will complain that it can't find the part file and asks you to identify it. At this point you identify the #2 part file. Inventor will continue opening the drawing and will save it with a permanent link to the new part file. Remember to set the #1 part back to the original name.

Inventor will also try to keep all dimensions that have the same origin. If you have - like you say - iParts then you have all the luck since for Inventor all variations of an iPart share the same geometry.

Alex

[mcgyvr]

Do you absolutely need the "bend direction" text? or would just a different color line be ok?

You can quickly save a dxf file directly from the part (ipt) file and can have the lines different colors for "bend down" vs "bend up"

To save a dxf press the "go to flat pattern" and right click on the flat pattern node in the model browser and select "save copy as".. Give it a name and make sure its set to dxf and then another dialog will pop up where you can set the color of the "bend down" layer to whatever color you want.. 

Doing this doesn't require you to make a drawing at all to be able to export a dxf file.. 

Here is an example.. Note the one bend (up) is a white line and the bend (down) is a red line..

You can also turn off tangent lines,etc.. or whatever you want.. 

[SBix26]

@alex.haerens Wouldn't the Replace Model Reference in Drawing tool be more efficient than changing file names?  I've certainly done it your way, especially back in the day before this tool was added, but it has made the process much less painful.

Manage Tab > Modify panel > Replace Model Reference in Drawing

Sam B

Inventor Professional 2017.4
Vault Workgroup 2017.0.3
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[alex.haerens]

"Replace Model Reference" ?

Well I'm working in IV2014 and that's a command that's not in. Good that it finally made it....  I celebrated the millenium change by starting my own sheetmetal design shop with Solid Edge and "edit links" was a command that had been there for years, and used on a daily base.

The bigger the company the slower the changes ? 🙂

Alex

[SBix26]

Hi, Alex-- look again, it's in 2014, too.  It was added in the 2011 release, according to the What's New document that I still have cluttering up my "bookshelf".

Sam B

Inventor Professional 2017.4
Vault Workgroup 2017.0.3
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[alex.haerens]

Surprise, surprise. Well, it was obvious and still well hidden in the same time. I think I would have expected it rather in the drawing view dialogue, where the model reference is shown.

Inventor still needs a broader link management. The one in place for drawings seems to be OK but there are other places where links are vital : imported solids could get exchanged, make derived parts refer to another source, link extrusions to sketches from alternate sources...  All this needs links that can be edited. If you can do it by fooling IV with missing part files you should be able to do it neatly with editing links.