Inventor General Discussion

Inventor General Discussion

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Distinguished Contributor
JimSteinmeyer
Posts: 326
Registered: ‎05-16-2011
Message 1 of 16 (1,248 Views)
Accepted Solution

dimensioning slots

1248 Views, 15 Replies
03-28-2012 07:08 AM

How do you go about dimensioning slots in drawings? In SW I would create the dimensions, edit the radius one to add SLOT at the begining and then select the length dimension to add it to the string. then the dimensions were linked to the part and not just dumb text. I am not finding a simular function here.

 

Thank you

 

Jim

Jim

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JimSteinmeyer wrote:

JD,

The only glyphs i seem to be able to get


 

This example is in ipt sketch - but works the same in drawing.

Watch when I select get near the bottom arc it changes to two different glyphs.

 

Slot Length.gif

 

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JDMather
Posts: 28,254
Registered: ‎04-20-2006
Message 2 of 16 (1,243 Views)

Re: dimensioning slots

03-28-2012 07:18 AM in reply to: JimSteinmeyer
Spoiler
 

Start the dimension command and select one of the arcs.
Then move your mouse around the second arc - near a quadrant you should get a special dimensional symbol.

If you click on th arc why this special glyph is displayed it will give you the slot length dimension.

Hollar back if you can't get it to work.

Please mark this response as "Accept as Solution" if it answers your question.
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Cadmanto
Posts: 3,356
Registered: ‎12-07-2011
Message 3 of 16 (1,238 Views)

Re: dimensioning slots

03-28-2012 07:24 AM in reply to: JimSteinmeyer

Jim,

Chek out my thread.

I asked a very similar question.

http://forums.autodesk.com/t5/Autodesk-Inventor/Tangent-Dimensioning-of-Arcs/td-p/3317169

Best Regards,
Scott McFadden
Inventor Professional 2014
(Colossians 3:23-25)

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jtylerbc
Posts: 898
Registered: ‎09-01-2010
Message 4 of 16 (1,237 Views)

Re: dimensioning slots

03-28-2012 07:31 AM in reply to: JimSteinmeyer

I usually dimension mine in a detail view that actually shows the length dimensioned, so I don't do it quite the way you're describing. 

 

It's an odd thing (that I'd never noticed before trying to answer this) that you can't insert parameters in the text of a dimension, but you can in leader text, and regular text.  The function you want DOES exist, just for some reason it doesn't exist for dimensions in particular.  If you really want to dimension it the way you're used to and keep it associated properly, I think the thing to do would be to "fake" the dimension with a leader text, and insert the parameters for both the radius and length of the slot.  Your text would look something like this:

 

SLOT R<Slot_Radius> X <Slot_Length> LONG

 

Where <Slot_Radius> and <Slot_Length> are the parameters you inserted from the drop-down lists.  When you're inserting the parameter, you can set number of decimal places it shows to the precision you want to show.

John Tyler
Inventor 2015
Windows 7 64 Bit
Distinguished Contributor
JimSteinmeyer
Posts: 326
Registered: ‎05-16-2011
Message 5 of 16 (1,217 Views)

Re: dimensioning slots

03-28-2012 08:32 AM in reply to: JDMather

JD,

The only glyphs i seem to be able to get are the radius one when I make the first selection and then no matter where I move the curser, or how long I hold it there the only glyph that shows up is for length dimmension. Is there something I need to turn on in the snaps?

Also in gooing over your tips section from skills university I see you reccoment not mirroring in sketches. I thought that would help when creating symetry. What is the reason for not mirring?

 

Thank you

 

Jim

Jim

Inventor Premium 2013 SP1.1
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Distinguished Contributor
JimSteinmeyer
Posts: 326
Registered: ‎05-16-2011
Message 6 of 16 (1,210 Views)

Re: dimensioning slots

03-28-2012 08:46 AM in reply to: jtylerbc

jtylerbc,

Your method is very simular to what I am accoustomed to doing. I just looked at this again and I think I see where you are talking about the pull downs, I need to select the part that is being dimensioned and then scroll through the dimensions to find the right ones. WOW. Since we place an assembly and then place and dimension components on following sheets This could be lots of fun.  In SW I would place one dimension then edit text and add the second by simply picking it. then hide the redundant dim. work done.

 

Jim

Jim

Inventor Premium 2013 SP1.1
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celeron cpu w\ 4gb RAM and 64 bit system
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Ya, my boss has me running my personal machine at work.
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JDMather
Posts: 28,254
Registered: ‎04-20-2006
Message 7 of 16 (1,205 Views)

Re: dimensioning slots

03-28-2012 08:52 AM in reply to: JimSteinmeyer

JimSteinmeyer wrote:

JD,

The only glyphs i seem to be able to get


 

This example is in ipt sketch - but works the same in drawing.

Watch when I select get near the bottom arc it changes to two different glyphs.

 

Slot Length.gif

 

Please mark this response as "Accept as Solution" if it answers your question.
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Valued Mentor
GSE_Dan_A
Posts: 311
Registered: ‎10-06-2011
Message 8 of 16 (1,194 Views)

Re: dimensioning slots

03-28-2012 09:00 AM in reply to: JimSteinmeyer

I typically point to the Slot with a Leader text and type its dimensions
ie (Dia) x (Length)

GSE Consultants Inc.
Windsor, ON. Canada
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JDMather
Posts: 28,254
Registered: ‎04-20-2006
Message 9 of 16 (1,192 Views)

Re: dimensioning slots

03-28-2012 09:03 AM in reply to: JDMather

For the other question why to avoid Mirror or sketch entities.

Open the attached ipt file.

On the left side I mirrored sketch geometry in the sketch/

In the right side I sketched the geometry myself and then added Symmetry constraint myself (could have just done tangent on this - but I'm trying to explain a simple example of what could be far more complex mirror).

 

Start the Extrude command and hover your mouse over different areas in the left - now do it in the right.

If YOU add the symmetry constraints rather than Inventor - Inventor finds more closed boundaries that you can use.  I would call this a bug - but it has been there for years. (Oops - I got both videos in this recording. I wondered why there was a black box around the second one.)

 

Avoid Mirror.gif

 

 

Please mark this response as "Accept as Solution" if it answers your question.
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jtylerbc
Posts: 898
Registered: ‎09-01-2010
Message 10 of 16 (1,183 Views)

Re: dimensioning slots

03-28-2012 09:09 AM in reply to: JimSteinmeyer

That would be a nice little shortcut, but I don't think you can do it currently in Inventor.  Probably one of the reasons it never occurred to me to dimension the slots I do that way - I just use a detail view and actually show the slot length and radius dimensions, instead of fiddling around with leader text.  But if I was going to, the method I described is the one I would use.

 

It's a bit clunky, but it's the best equivalent I can think of to what you're trying to replicate from SW.

John Tyler
Inventor 2015
Windows 7 64 Bit
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