Inventor 2014

[ashutoshighe]

Hi guys...

Pls let me know how to place the section view as base view while drafting in inventor 14,  that mean how would i place the section view directly as new......

Ashu

[harco · Accepted solution]

Not possible.

Inventor needs to know where to section and this comes from the parent view.

Create the base view, then create the section from the base and drag the base view off the sheet onto grey space leaving the section on the sheet.

The base view will not print as long as the print settings are correct.

You might possibly be able to create base on one sheet and drag the section onto second sheet but it will still need a parent view.

[blair]

As Harco stated, you need to have a "View" to Section. Rather than dragging off the screen into Grey-Space. Just RMB on the desired view and select "Suppress"

[ashutoshighe]

Sir, Thanks for a reply..

Pls tell me, any other easy solution, whether is it possible to make
section in part and same will be placed in the drw file..
also let me know this command, here i am sending you screen shot..
all command how will i operate???[image: Inline image 1]

[ampster401]

no screenshot was attached - but like others have said, there is no way to create a "section view" inside a part file and then be able to bring that into a idw drawing.

You have to create a base view first, then create the section view.  If you do not want to see the base view, you can slide the view outside of the titleblock border so it won't print as harco stated..

That is your only option.

[-niels-]

The only other way i can think of for making the base view sectioned is to add a "break out" to it.

There is no direct way, either make a section and hide or suppress the base or add a break out to the base...

[ampster401]

if you don't mind destroying the part file, or perhaps don't mind creating another part file so you do not destroy the original is to use the Split command on the part being careful to Split it at the exact location you need a "Section view" of.

Then when you bring that Split part file into an idw or dwg drawing file, you can just create a single base view using the Split surface as your base view.

However doing it this way, you will have to add Section Lines (hatching) manually if you need the view to appear as a Section View.

Hope that makes sense.

[blair]

Or place in into a IAM file and use the Assembly Tools to Cut the part. The Original will still be intact but you will have a cut part only in the IAM file. Then use it for your drawing view. If possibly, save the IAM file with the same name as the IPT. It will have a different file extension name but will be easy to identify.

[ampster401]

as you can see by the replies, there are "ways around this"...

But why "fight" the software?  Just go with the flow with how the software has been designed and you should be able to get by without having to do so much rework.  What I'm getting at here is the simpliest method would be to just insert a base view and then create a section view from that and hide the base view outside the border since it sounds like you don't want it.

[ashutoshighe]

Dear Mr. ampster

First of all thanks for the soultion.. I just wanna know the simplest method for section view.. If it is not, no problem, I m using same regular method.

Also i request you to pls find the attachment and explain me all these feature, which will be usefull for me..

[blair]

That only for secondary views based off the Primary View. It's not what you are looking for. The section is only active on a view projected from the base view. Follow one of the 3 suggestions. 1.) drag the Base View off the page into the "Grey" area. 2.) Suppress the Base View after you have done your Section View. 3.) Create a new IAM file, place your IPT into the IAM and use the Assembly Tools to create an Extrusion to cut the IPT. It will only be "Cut" in the IAM file. It won't affect your IPT file. Then create a drawing using the IAM as your source. It will come in "Cut"