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Creo 7 MBD - how to annotate the Pitch Circle Dimension

Seth
4-Participant

Creo 7 MBD - how to annotate the Pitch Circle Dimension

Dear All,

 

I am converting a 2D drawing from a part of an existing product into a MBD dataset. To do so, I would like my MBD dataset to fully encompass all the annotations found in the 2D drawing (as they are the critical dimensions of the part), however, on the 2D drawing a Pitch Circle Dimension (PCD) of a hole pattern has been specified. I tried to annotate this through selecting 'Show dimensions' on the holes that lay on the pitch circle, but this did not work. Furthermore I tried 'Dimension' from the annotations tab but this also seemed to not be able to show the PCD. On both PTC (community) website and Google I could not find any answer on how to do this correctly, so therefore I am posting here.


My question is: How can I (3D) annotate the Pitch Circle Dimension?

 

I did find a small work around, to use 'dimension' between two holes of the dimension. This sort of gives the dimension of the PCD, but the two holes are not parallel to the x-axis of the annotation plane. Skewing solves this and makes it parallel but then the leader lines are not equal length, resulting in the dimension text being angled compared to the x-axis of the annotation plane. Furthermore I doubt if this gives correct data that can be used downstream.

 

Thanks in advance,

 

Seth

1 ACCEPTED SOLUTION

Accepted Solutions
pausob
16-Pearl
(To:Seth)

MBD combined state: showing feature and part dimensions (Creo 4):

radial_pattern_pcd.png

Note: patterned hole defined using "radial" (or "diameter") placement.

 

View solution in original post

6 REPLIES 6
MartinHanak
23-Emerald V
(To:Seth)


@Seth wrote:

Dear All,

 

I am converting a 2D drawing from a part of an existing product into a MBD dataset. To do so, I would like my MBD dataset to fully encompass all the annotations found in the 2D drawing (as they are the critical dimensions of the part), however, on the 2D drawing a Pitch Circle Dimension (PCD) of a hole pattern has been specified. I tried to annotate this through selecting 'Show dimensions' on the holes that lay on the pitch circle, but this did not work. Furthermore I tried 'Dimension' from the annotations tab but this also seemed to not be able to show the PCD. On both PTC (community) website and Google I could not find any answer on how to do this correctly, so therefore I am posting here.


My question is: How can I (3D) annotate the Pitch Circle Dimension?

 

I did find a small work around, to use 'dimension' between two holes of the dimension. This sort of gives the dimension of the PCD, but the two holes are not parallel to the x-axis of the annotation plane. Skewing solves this and makes it parallel but then the leader lines are not equal length, resulting in the dimension text being angled compared to the x-axis of the annotation plane. Furthermore I doubt if this gives correct data that can be used downstream.

 

Thanks in advance,

 

Seth


Hi,

I guess you have to create additional Sketch feature containing circle.


Martin Hanák

This may be related to how the holes were created in the model. If you post the part or a simplified model with the holes created exactly (copy/paste from one model to another) as in your model that will allow for investigation.

 

If you used a pattern for the holes what is the dimensioning scheme for the pattern lead? Does the lead hole include a  diameter dimension?

pausob
16-Pearl
(To:Seth)

MBD combined state: showing feature and part dimensions (Creo 4):

radial_pattern_pcd.png

Note: patterned hole defined using "radial" (or "diameter") placement.

 

View solution in original post

Seth
4-Participant
(To:pausob)

Hi, I wanted to thank you (and the rest) for the helping. This ended up working. The only thing I can not get to show yet is the circle itself (the -. circle in your picture).

pausob
16-Pearl
(To:Seth)

Not sure why the PCD circle display doesn't work for you.  In Annotate mode, I select the patterned holes, right click and "Show annotations"

There used to be a setting called radial_pattern_axis_circle and it has to be set to YES for the circle to show up, but I don't see it in Creo 4 anymore.

Seth
4-Participant
(To:pausob)

Hi Pausob,

 

I figured it out, some hole patterns in my part did show the -. circle but not all. I found that it depends on how the hole pattern is defined. If the original hole is defined within an extrude the diameter of the circle on which it lays is not set during creation of the hole, resulting into the PCD -. circle not showing. If I create a hole, selecting a surface as placement and axis + plane as offset I do have to fill in the diameter of the circle on which it lays, if I then click show annotations the PCD -. circle then does show.

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