dimensioning slots

[JimSteinmeyer]

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

[JDMather]

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.

[Cadmanto]

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

[jtylerbc]

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.

[JimSteinmeyer]

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

[JimSteinmeyer]

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

[JDMather · Accepted solution]

---

@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.

[GSE_Dan_A]

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

[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.)

[jtylerbc]

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.

[JimSteinmeyer]

JD,

Interesting, I was finally able to get the glyph to show  but it only gives me the dimension of the segment between the arcs. maybe the difference is due to my having  arcs and not circles. I will keep playing with it and will probably get it to work with practice.

Thank you for your help.

Jim

[JimSteinmeyer]

JD,

It does look like the symetry command will be my friend from now on.

Thank you

[Rich.O.3d]

---

@jtylerbc wrote:

...that you can't insert parameters in the text of a dimension,...

---

hmmm...

On the edit dimension box, there is a button with a pencil on it.

If you click that, then you go to the text editor box.

In the text editor box, you can pick the part and the paramater that you want to show in the dimension.

You may be confusing with iproperties, which you cant pick for dims.

[jtylerbc]

You're right - my mistake.  Not sure how I was missing that, since I use it all the time in view labels.  Thanks.

So, Jim,  you can follow my previously posted method in a radial dimension, if you click the pencil icon first to get to the full text editor.  Doing it that way, you'll only have to insert the parameter for the length, instead of both radius and length.  Should take some of the pain out of it.

[JimSteinmeyer]

Thank you. It seems a long way around the barn to get something done, but at least we can do it.

Jim

[Rich.O.3d]

this functionality should be added into the hole note tool

after all slots are considered to be elongated holes

I set the dimension names to slot_width and slot_length (refer attached) as I create them.

This makes it easier to find them when you create your leader note or dimensions.