Ordinate Diameter Dimensioning

[CGardner01]

I design molds for the rubber industry and I was using Acad 2000; I am just now starting to use inventor. I need to used the ordinate dimensioning although I need the dimension to be given as a diameter and not as a radius. Is there anyway to scale the ordinate dimension automatically as 2:1? This way when I give the prints to the tool room they don't have to manually double every diametrical dimension. The prints that I draw only show half of the mold, there for needing a 2:1 dimension scale.

[harco]

RMB after selecting dim and set type to diameter.

[ob1966]

If you use ordinate dimension tool (not the ord dim SET tool) then you can create you dims, point to the origin indicater, RMC and "move the origin to the desires offset value (2:1 in your case).

[CAGardner01]

Thanks for the input, although I have not got it yet. When I select an ordinate dimension and right click there is no "OPTIONS" to select in order do set the type to Diameter. Just by moving the origin doesn't give me true diameter readings, except the one that you set the origin position from. Please continue to give input so that I can figure this out. Remember that I am totally new to this program so please explain in detail. I am assuming that RMB and RMC both mean "right-click"? Thanks for your help.

[mcgyvr]

What does ordinate dimensions have to do with hole radius/diameters? You can't place dim or rad dimensions with ordinate dimensions... (or did I miss some trick along the way??)
Use the regular dimension or Hole note command to place diameter or radius dimensions. Also if its a full circle it will place a diameter dimension if its not then it should't have one and should put a radius.

[Anonymous]

You did not miss anything.... although, there ARE quadrants.. 🙂
--
Dennis Jeffrey, Autodesk Inventor Certified Expert
Autodesk Manufacturing Implementation Certified Expert.
Instructor/Author/Sr. App Engr. Tel. (260) 399-6615
http://teknigroup.com

[CAGardner01]

You did miss something. You are right that you would not use ordinate dimensions for holes. I am not talking about holes. For example, I am drawing a mold half (say the bottom plate). That bottom plate is 30 inches in diameter and there is a cavity that molds the rubber to that cavities shape when the top and bottom plates come together under heat an pressure. Now the dimensions to that cavity (lets say that it is a groove) are .125 x .0625DP, and the grooves ID is 28 inches. So I place the 30 inch diameter plate into a drawing and the plate is so large compared to the cavity that you can even see the cavity. So I make a section view (cutting the mold plate in half) and then from that I make a detailed view of the cavity (scaled several times larger). Now on that detailed view we use ordinate dimensioning to show every detail such as the starts and stops of radii and etc. We dimension in diameter, which makes it much easier for our tool room. I have attached an AutoCAD drawing describing how we dimension our molds.

[mcgyvr]

I made comments about not being any ordinate dimensions shown on that drawing.. I have edit this post because... Now I see your small drawing. I didn't zoom all the way out.

Edited by: mcgyvr on Sep 4, 2009 12:09 PM

[mcgyvr]

Now to answer your question. No you cannot. Why. Thats just not how ordinate dimensions should work. It is not inline with any dimensioning standards which Inventor complies with. Autocad allows you to fudge anything you want (right or wrong). Now here is where I step out because I am far from the dimensioning expert and don't have any good ideas on how to detail and dimension that type of feature in Inventor. Good luck finding a solution.

[WayneTaylor]

This is why inventor is not as good as solidworks.

[SBix26]

That's it? That's why?  Since we never need this capability, I guess we made the right choice!

[kiefer.dunham]

I realize this thread is ancient in terms of inventor, that said this is for anyone who more recently has had a similar issue. I often draw revolved parts with various changes in diameter. This requires a lot of dimension lines and detail views to illustrate the smaller geometry clearly. My solution to this is to do a half section view of the revolved part, hide the geometry on one side the center line and scale up the section view. While I have not found a way to change the ordinate dimension tool to represent a diametric value when the origin is placed at the center, I can explain a similar method that should prove just as useful. 

1. Select the general dimension tool

2. Select the geometry that you would like the extension line to start from

3. Select you center line (draw a center line first if you have not already)

4. Right click and select dimension type from the drop down menu

5. Select linear diameter from the second drop down menu

6. Drag you dimension to your preferred location 

I hope this helps.

[ian]

Ok, so I have a cross section of a turned part, my zero point is the axis, I want to dimension start & end points of arcs, intersections etc.

The PDF attached, I have had to manually change from rads to diameters, I was hoping to RMB,  and get the dimension type option (radius or diameter)

[johnsonshiue]

Hi! I am not sure if this is related. Here is a frequently overlooked option in Tools -> App Options -> Drawing -> Dimension Type Preferences. You may select the desirable types so that you don't have to keep changing the type when creating a new dimension.

Many thanks!