unable to pick a point while dimensioning with chain dim. command and ordinate dim

[Rishi-Bhardwaj]

Dear All Inventor Users,

                                                there is a problem with ordinate and chain dimension tool in inventor drawing environment.

Inventor works very smoothly with drawings & it highlights all the points when, I move my cursor on it, It highlights  center point of arcs and circles. But while dimensioning with chain or ordinate dimension tool, it doesn't  highlight center points and midpoints. And problem arises when, I have to add dimensions  from a certain point to the center of slot. 

I have also attached a screenshot for reference here.

If there is anything that, I should know, Please let me know. 

Thanks in Advance.. 

[SBix26]

See if this setting helps:

Better yet, post your files here so we can better understand what's happening.  Slots do not have an automatic centerpoint in Inventor, but you can pretty easily add one in the model, then include it in the drawing for this purpose.

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[Rishi-Bhardwaj]

No, this doesn't works for me.

[rogmitch]

Generally you will find that features that are not accessible whilst initially placing the ordinate/chain dimensions become accessible when using the 'Add Member' option on the right click menu.  I do not understand why the  dimension tool works in this way.

RM

[Rishi-Bhardwaj]

sir, i didn't get your point, can you please elaborate little bit more.

[rogmitch]

Just try and dimension a simple block with a slot through it using 'Ordinate Set' dimensions.  You will find you cannot pick the midpoint of the slot edge only the two ends of the block itself. 

Complete the 'Ordinate Set' with just the block edges, then right click on those dimensions and pick 'Add member'.  You will now be able to pick the midpoint of the slot edge. 

RM

[SBix26]

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@rogmitch wrote:

Complete the 'Ordinate Set' with just the block edges, then right click on those dimensions and pick 'Add member'.  You will now be able to pick the midpoint of the slot edge. 

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Or select the set, then drag the attach point of an existing member to the slot midpoint.  Saves deleting unneeded ones later.  But I wonder why you can't pick the midpoint of the slot edge?  I can on Inventor 2023:

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[johnsonshiue]

Hi! What release of Inventor are you using? Please share the files here. We do have an issue in 2023 or 2022.3.

Many thanks!

[rogmitch]

Hi Johnson,

I am using 2022.3 at present.  I have not tested whether it works in 2023 yet.   

It is something I have noticed over other releases going back many years but I have never heard anyone else mention it.

I attach my simple part that shows the effect in 2022.3.

Thanks

Roger

[Rishi-Bhardwaj]

I have attached a dwg. file for reference here & Currently, I am using Inventor 2022.

[johnsonshiue]

Hi! Many thanks for sharing the files! They help me understand the issue and the requirement better. Scratch my prior comments. Those are irrelevant. This is about dimensioning slot center in the drawing, regardless of dimension types (Chain, Ordinate or Regular).

It is true that there isn't a dimensioning workflow that snaps to the center of a slot. To facilitate the selection, you will need to create such center. The centerline tools can help.

Use Bi-Sector tool -> pick the two arcs of the slot. Repeat it for the parallel lines. Now, the slot center is created. Any dimension tool can pick up.

Thanks again!

[Rishi-Bhardwaj]

Sir, Thanks for your reply. For better understanding, I have attached a screenshot here. In normal case I can pick a center point of line of slot. that is fine, it works for me. But with Chain or Ordinate dim. it doesn't allow me to do that.

If there is any else that, I should know. please let  me know. Thanks again

[rogmitch]

Hi Johnson,

You mentioned in your post  'It is true that there isn't a dimensioning workflow that snaps to the center of a slot'.  

Another option to creating bisector lines is to use Baseline, Chain or Ordinate Set.  Once you place a dimension set on the drawing view the slot centres become available via 'Add Member'.

RM

[johnsonshiue]

Hi @Rishi-Bhardwaj,

In your case, you could use Sam's workflow. I thought you needed to snap to the exact center of the slot. Basically, to enable midpoint selection in Ordinate or Chain dimension, you need to uncheck the following option.

Tools -> App Options -> Drawing -> "Enable ordinate dimension geometry selection".

Once it is unchecked, the midpoints will be selectable. Please try it out.

Many thanks!

[Rishi-Bhardwaj]

it doesn't help me to get out of this situation.

may be, I am not doing it in a right way. 

[johnsonshiue]

Hi! I am sorry I got confused again. Chain dimension behavior is not controlled by "Enable ordinate dimension geometry selection" option. We may have some regressions in recent releases. But, here is how it is supposed to work.

Chain Dimension: The ability to select a midpoint isn't controlled by any option. You are not allowed to select a midpoint as the first pick before a legitimate dimension has been established. Pick a straight edge -> right-click -> Continue -> now you are allowed to select a midpoint or any vertex to chain the dimensions. Virtual sharps are not supported.

Ordinate Dimension: The ability to select a midpoint or any vertex on the first pick is indeed controlled by "Enable ordinate dimension geometry selection." With this option on, only an edge or edges can be selected on the first pick. But, after the first pick and an ordinate dimension is created, any vertex can be selected to create subsequent ordinate dimensions.

With the option off, you are allowed to select any vertex or a virtual sharp anytime within the command.

Many thanks!

[Rishi-Bhardwaj]

Sir, can you please attach a screenshot for better understanding. I think, I didn't get your  point yet.

Please help me to understand.........

[Rob_Windsor · Accepted solution]

If I am following this correctly, there is a specific step-by-step that you need to follow, as there are specific rules that have to be followed:  

start your ordinate/chain dimension,

click on the start edge of the plate/sheet

click on the end edge of the plate/sheet

right-click, Continue

now you can click on the midpoints to add your slot midpoint dimensions,

right-click, Create

I tested this out myself.  Once you start the Ordinate/Chain dimension, it only lets you click on geometry like lines & circles.  So, you click on the start line and end line.  Once you right-click, continue, place your dimensions, now you can click on end points and midpoints to add more dimensions.  Don't forget to right-click, create at the end of it all.

<iframe width="640" height="590" src="https://screencast.autodesk.com/Embed/Timeline/d63b82f4-e193-4875-bec0-a24e1857a6b4" frameborder="0" allowfullscreen webkitallowfullscreen></iframe>

It looks like I need a tutorial on how to imbed a video...  LOL  Tips?

[SBix26 · Accepted solution]

That's how it works for Chain dimensions, but Ordinate dimensions are a bit different.

As various of us have tried to describe in previous postings in this topic, Ordinate dimension selection behavior depends on the status of the Application Option Enable ordinate dimension geometry selection:

• When checked, points are not available to be selected when initially placing ordinate dimensions, though they can be selected later by adding members or dragging existing ones
• When unchecked, points (including mid-points) are available to select for dimension placement

I hope that helps clarify this.

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Sam B

Inventor Pro 2023.0.1 | Windows 10 Home 21H2

[Rishi-Bhardwaj]

Thanks to all of you. This is what  makes Inventor Strong.

Again Thanks to all of you.