Measure Distance From Midpoint to Midpoint of Edges

[buser]

Hi Community,

I'm new to this forum so please be gentle. Currently using Creo 2.0

Quite often I want to measure distance from a midpoint of an edge in a feature/part to a midpoint of an edge in another feature/part. The distance is to be projected to a common parallel plane/surface. The edges may or may not be in the same topology. This shouldn't be rocket science.

Went thru all the filters in the analysis > measure distance mode and no luck. It would be great if the analysis tool would allow you to snap to the midpoint of an edge when you activate the edge filter. Hint Hint PTC

So the only way I'm able to achieve such measurement is to create a sketch on a parallel plane/surface where I project the edges of interest as curves. I then add center construction lines and midpoint-constrain them to the projected curves. (get it? midpoint constrain?) I then add a ref dimension.

I've added some screen shots to explain the scenario better.

Is there a less rookie way to do this? I really want to avoid going to sketch mode every time and would like to achieve this measurement in, you know, the measurement tool.

Thanks

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[dgschaefer · Accepted solution]

While in the measure tool, you can create datum features on the fly to assist in your measurements. So, you can create a point at the midpoint of edge 1 and another at the midpoint of edge 2. The nice thing about this is any datums you create while measuring are temporary and will be removed once you exit the measure tool.

There's also a projection reference tool within the measure dialog to show the distance as projected on a plane or, if you pick a CS, it'll give you the X, Y & Z distances.

[dgschaefer]

Also, add "measure_dialog_expand yes" to your config.pro to force the measure dialog open by default.

[buser]

Thanks Doug,

I appreciate your comment.

Can you please elaborate what I need to click to create datum features on the fly while in measurement tool?

When I tried it (while in measure tool), I selected the create point button under the datum tab. I then created the two points and it let me measure but when I exit the measure tool, the points remained in the feature tree.

Thanks

[JLG]

There is a config.pro option that controls whether the points are temporary or not -- keep_info_datums. I'm guessing you must have it set to yes, the default value. Set it to no and the points created during measurement will be temporary.

[dgschaefer]

Yes, that's it. I had forgotten about that option, I set that option to no to prevent my model from filling up with extra points and planes.

[buser]

Yes, that's it!

Thanks for helping me out with this

[BuddyHudson]

Hey Doug,

I am not seeing where you can create a datum on the fly while in the measurement tool? Mine are grayed out when I measure....???

Can you clarify?

Thanks,

Buddy Hudson

[BuddyHudson]

Ooops! My bad, I had the part locked in my workspace in Windchill. I have them now.

Sorry Doug.