How can I draw this goove

[097013309]

Anybody can show me how to draw this groove from blueprint please.

[JDMather]

Looks like a Revolve - Cut to me.

You attached an iam (assembly file).

That drawing looks like it should be an ipt (part file).

An assembly file (*.iam) is only a list of hyperlinks to the part files (*.ipt) and a record of assembly constraints (and a bit more).

You must include the part files.

[097013309]

In the process I probably open it in the assembly and save it as assembly file ( *.iam) and lost my part file ( *.ipt) can this  be revers?

Can you elaborate about in little more then (Revolve-Cut) so I can draw it please.

[Pauli666]

You dont say what version you are running, here is revolve & extrude example (Can be accomplished in more ways i am sure) using IV2013

[JDMather]

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@097013309 wrote:

In the process I probably open it in the assembly and save it as assembly file ( *.iam) and lost my part file ( *.ipt) can this  be revers?

Can you elaborate about in little more then (Revolve-Cut) so I can draw it please.

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You cannot save a part file as an assembly file.

Your part file name is Hinge_Mount.MCNEIL.IPT search your hard drive.

I recommed that you first learn how to set up a project file (*.ipj)
I recommend that you put this aside for a while and go through these

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf
http://inventortrenches.blogspot.com/p/inventor-tutorials.html
http://wikihelp.autodesk.com/enu?adskContextId=HELP_TUTORIALS&language=ENU&release=2014&product=Inve...

[097013309]

I am running Autodesk Inventor Professional 2014 Student version.

I can't open your file. When I click on attachment Inventor opening it ,but nothing on the screen or browser.

Thank you for answer.

[097013309]

Ok. I find my file  and I am attachung itI stiil need advice how to do this groove. Do I should make costruction plane firs? I need surface to put drawing on it ? How I can "go Inside hole" to be able to draw it?

[097013309]

I find file on the stick. I am attaching it but still need some help. Just tell me seps please.

[conklinjm · Accepted solution]

Unfortunately I have an older version of Inventor and cannot open your part; however, I shall try and answer your question.

Yes, depending on how you created the original sketch, you may need to create a construction axis and work plane to create the revolution.

If the original sketch was on the XY plane and the large bore centered at 0,0, you could sketch on the YZ plane.  One method is  ...

1) Create a new sketch on the YZ plane

2) Project the Z-axis

3) Draw beneath it a parallel centerline

4) Dimension between these two lines (i.e. 4.0 in)

5) Sketch the revolution (should take ten lines -- X.XX x 0.125 / 1.130 x 0.056 / X.XX x Y.YY / 0.933 x 0.125 bore)

6) Apply three diameter dimensions using the centerline (i.e. X.XX, 1.130 & 0.933)

7) Apply collinear constraint between the two X.XX line segments

😎 Apply three length dimensions (i.e. 0.125, 0.056 & 0.125)

9) Project either the top / bottom edge of the raw material or the two ends of the larger circular bore

10) Constrain the two ends of the revolution to either the end points of the projected edge (line to point) or the two circular projections (collinear lines);  Note that the length Y.YY is not needed to be dimensioned as the bore will automatically adjust to the width of the raw material due to these projected elements & constraints

11) Finish Sketch

12) Revolve using the cut option

13) Choose a circular Array

14) Pick the Revolution as the 'Feature'

15) Pick the Z-axis as the 'Axis'

16) Set the number to 3, the angle to 60 and the style to dual-direction

HTH

- - - - - - -

Not sure from where the drawing you are using came but, to completely recreate it, you require more information as many dimensions are missing (such as the size of the bore shown as X.XX above).

[JDMather · Accepted solution]

Open the attached file.

Find the red End of Part marker in the feature browser.

Drag the red EOP marker down feature-by-feature and examine how they were created.

The Revolve feature is one technique.

You should place the origin for the part at the same location as the origin for the ordinate dimensions.

Note that my part sketches are fully defined.