Retrieve Dimensions in IDW

[dcmorgan]

Hello All.

I currently design and manufacture tons of replacement parts of all shapes and sizes for meat grinders. I am stickler for trying to have as much information come directly from the model rather than manual inputs in the idw which can turn into a nightmare quickly when managing files and keeping info correct between variations of each part. With that being said, I really like retrieving dimensional tolerances from the model whenever I can. The problem is that I am still able to edit these tolerances in the idw.

Is their anyway I can retrieve tolerances from model and have them be grayed out in the idw. I use a lot of deviational tolerances which may pose a bigger challenge then using standard symmetrical ± tolerances.

Any thoughts would be greatly apprciated!

Dan

[lesmfunk]

Maybe ditching the idw would be an option for you, if Autodesk ever gets there. (I'm talking about PMI or MBD. SW launched theirs this year)

[mcgyvr]

I'm not aware of a way..

Personally this should be handled by company policies/training.. Just stop changing the tolerances in the drawings..

There is this in application options..drawing tab 

Enable part modification from within drawings

Enables or disables part modification from within drawings. Changes to a model dimension on a drawing change the corresponding part dimension.

But frankly I don't even know how that works if it does..

You would "think" thats the setting you are looking for but it doesn't seem to do anything for me ..checked or unchecked..

[salariua · Accepted solution]

In general all the recommendations are to use drawing dimensioning and tolerancing functionality. The assembly tolerances are mainly used in interference check, stack-up etc. I do use them in parts trying to maintain the design intent especially when cloning and copying parts.

This is a bug.

Retrieved dimensions should be editable (value and tolerance) only via right-click Edit Model Dimension. If you want different value or tolerance then place a dimension in the drawing which is a cosmetic feature.

Right now you can specify different tolerances by regular edit dimensions and override the model value which is not correct for a retrieved dimension.

Except for the existence of Edit Model Dimension option in the contextual menu there’s nothing to tell you that the dimension is coming from model and a user will edit it by fast-convenient double click.

The EVEN bigger bug is that with Edit Model Dimensions you can modify parent of derived part  

Normally parameters driven into other parts can only be modified in the parent part. I say ... normally.

[salariua · Accepted solution]

@mcgyvr wrote:

Enable part modification from within drawings

But frankly I don't even know how that works if it does..

You would "think" thats the setting you are looking for but it doesn't seem to do anything for me ..checked or unchecked..

---

If you uncheck the box for "enable part modifications..." you will not have a "edit model dimension" menu on right-click. that is ... if the dimension is retrieved from the model.

[mcgyvr]

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@salariua wrote:

@mcgyvr wrote:

Enable part modification from within drawings

But frankly I don't even know how that works if it does..

You would "think" thats the setting you are looking for but it doesn't seem to do anything for me ..checked or unchecked..

---

If you uncheck the box for "enable part modifications..." you will not have a "edit model dimension" menu on right-click. that is ... if the dimension is retrieved from the model.

---

Ah yes.. thanks..

NEVER used the RMB edit model dimension before..

Was sort of expecting different functionality but I got it now.. Thanks

[salariua]

Whenever I can i use the model dimensions because I can modify them from the drawing not needing to open the model, locate the sketch, edit sketch, finish edit, save, close part.

Sorry for detouring the post...

Back to you moderators and AU friends that have all the insides to help us out.

Are we doing the right thing here?

Is this how it was intended?

Is this a bug as we believe it to be ?

[salariua]

There's a Select Model Dimensions in the filter dialog and it will do just that , selects all dimensions retrieved from the model (extra way of telling which is model and which not).

The Select all Overridden dimensions only selects dimensions with "Override Displayed Value" checked.

I think we need an extra option that will select all modified dimensions and further more we need to have in the contextual menu, restore default or similar to remove all overrides, on dimension value, in text, in tolerances, and inspection tab options.

I think on a long shoot you can use the Select all Model Dimensions and then use delete to remove them all and then use retrieve when you think a drawing might have overridden values. 😞

[lesmfunk]

To bring this back to the original question, there are many offices where the engineers and designers only work in the 3D environment. Then detailers or drafters create the idw's (or slddrw's). If the engineers have defined the tolerances in the model, we don't want the detailers to be making changes in the idw (or worse, the model. Anyone who uses the Override Displayed Value deserves a good spanking!).

As Dan and Adrian have pointed out, Inventor has no way of preventing this.

I'm still curious to see how MBD deals with this.