How to change the number of decimal places for all model dimensions

[tbraxton]

I want to change the display of all dimensions in a previously built model to 3 decimal places in part mode.

PTC support documents the following steps to do this. I follow until step 6. Where is there a format tab and column in part mode? Menu mapper is not finding it and doc search is not fruitful. Can anyone elaborate on step 6 below?

In Creo Parametric 3.0 and later versions:

• 1. Ctrl+F or Tools > Find
  2. Set Look for and Look by to Dimension
  3. Click Find Now
  4. Click in the items found area and click Ctrl+A to select all dimensions
  5. Click the arrows icon to transfer items from items found to the Items Selected section of the Search Tool dialog box > Click Close
  6. Change the Decimal Places value as desired in Format column in Format tab

[TomU]

In Creo 6 it would be the 'Dimension' tab, but I'm have trouble getting it to appear just from the search results.  Even if I select one dimension and get the tab to appear, searching for additional dimensions and adding them to the selection set makes the tab disappear.  Hmmm...

[StephenW]

I'm on Creo 4.

When I finish step 5, it shows me all the dimensions and automatically shows the "Dimension" tab and I can set the # of digits there. I don't see a format tab either, at least not in Creo 4.

[TomU]

I believe the dimension tab replaced the format tab.  PTC probably just hasn't kept the article up to date.

[kdirth]

In Creo 4 I can select any or all dimensions and will get the dimension tab unless something in the model is suppressed.

I don't see a way to limit the Find feature from finding dimensions in suppressed features.

[kdirth]

I have found that, for whatever reason, precision (the section needed) is greyed out when an angle is included in the selection.  Looks like a program bug.

[tbraxton]

I just tested this and if the part has any angular dims the dimension tab is not activated or displayed. I am in Creo 4 M110 testing this. Creo 7.0.3 is also not working correctly, I just opened a case with support. I will post the response here when it comes.

[tbraxton]

I was wrong about angle dimensions being problematic. Any model which has dimensions in pattern features will not activate the dimension tab in Creo 4 M110 or Creo 7030 when following the process in the original post.

[tbraxton · Accepted solution]

The root cause of why this process was not working for me is that I was including pattern members in the find tool selection process (step 5). If any pattern members are selected that do not have dimensions then the dimension tab will not activate. This is intended functionality according to PTC.

The work around is to not select any pattern members in the find tool for selection (in step 5) then the dimension tab will be available and you can set the number of decimal places to be displayed. You can include pattern leaders that have a dimension in step 5 and it will still work but you need to insure that there are no features without a dimension selected in step 5.

[TomU]

I also opened a case to push tech support to update the article.  The whole point of the middle section is to update *ALL* model dimensions.  If there are certain types of dimensions that mess up this process (pattern members, suppressed, angular, etc.) and prevent display of the 'Dimension' tab, then the article needs to explain how to adjust the search results so these aren't inadvertently included.

[tbraxton]

I spoke with support earlier today. I provided the article # when I opened a call last week and they committed to updating it and adding information about features without dims to the article.

[pausob]

Hi, I'm late contributing to this thread as this is already marked as solved.
Anyway, I'm using Creo 4, and things seem to work fine, so I post a video that demonstrates the use of the Search tool for bulk-modifying properties of model dimensions.

Summary: I don't see problems in selecting the angular dimensions or dimensions that belong to pattern members.  The video also shows how you can modify the search query so that dimensions belonging to suppressed features are omitted from the results.

[tbraxton]

Both of your table patterns will have dimensions associated with each member. I suspect the dimension pattern also has a dim associated with each member. If this is the case that is why you are not replicating the issue. Try it with a dimension pattern where only the leader has a dimension and you will replicate the issue. If any item in the selection does not have an explicit dim assigned to it, the dim tab will not activate. 

[pausob]

The search procedure results in a bunch of dimensions being selected - so I don't understand this conclusion:

---

@tbraxton wrote:

issue. If any item in the selection does not have an explicit dim assigned to it, the dim tab will not activate. 

---

Ok, so in my video example the dim pattern had the holes changing in size.

So I redefined this pattern and removed that 2nd increment dimension; So only the leader has a diameter dimension.  The search procedure resulted in these dimensions being selected:

and as you can see, the dimension tab is available...

[tbraxton]

Upload the part you are testing, I may be able to put it context. The issue exists and PTC support is able to replicate it among others here who have responded. It is possible that it has something to do with config options I suppose which could result in different behavior.  PTC support did look at my environment when testing but perhaps they missed something.

[pausob]

Creo4 model attached.

[tbraxton]

Try it with this part (Creo 4). Are you able to access the dim tab when selecting all dimensions of this model? If any of the pattern dims are included in the selection of the search tool then the dim tab is not accessible when I test this. If I eliminate the pattern dims from selection then the dim tab is available.

[pausob]

Right, your model does not work.  And you were using an axis type of pattern.

So seems that only dimensions from pattern table or dimension based patterns can be modified.

[pausob]

I think I found a workaround:

1. Open the model in a new blank drawing

2. Set the detail option to allow_3d_dimensions

3. Create 1 general view in default orientation

4. Show all model dimensions on this view

5. Use the search tool procedure, in drawing mode and with the "search submodels" checked.

6. After this, the dimensions tab is available for bulk-change of the selected dimensions.

It seems the search results in the drawing mode filter out those ghost dimensions that tag along with copied features.  I suspect those show up in the sheetmetal models.

note also that the search tool in the drawing mode does not find the dimensions of suppressed features.

PTC should probably fix the part mode functionality to make the MBD work easier...

[tbraxton]

I tried this on one of my test parts and it works. A bit clunky but it is certainly a workaround for now. I would certainly vote for a product "improvement" to address this. I think that you should be able to make the global dimension selection in part mode when implementing this process.