sketched datums

[nrollins]

Hi all,



I am trying to sketch a point and get a datum axis to show up. I found this
in the Creo help:







Do you see the "the entities appear on the model tree" ??? What is that? I
am missing something really obvious, right?



Sketched entities in the model tree? I have never seen that. Anyone out
there has?



Anyway - maybe you can tell me WHY I cannot get a sketched point to generate
a datum axis - like I have a thousand times before. Today it doesn't want
to work. I must not have my framis turned on or something.



-Nate


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.

[DonSenchuk]

In sketcher there are two different icons to create a point. One creates a point just in the sketch to be used for references or constraints. The other point results in a datum axis.

Red circle = datum axis point
Blue circle = sketcher only point

[cid:image002.png@01CF7A48.3503F700]

You can also pick any existing point, RBM and switch it between Construction (no axis) and Geometry (axis).

The one caveat in all this is if you're creating a Sketch feature instead of working on a sketch embedded within another feature (like an extrude). In that case the Geometry point results in a point (tied to the sketch) visible when point display is turned on, while the Construction point results in nothing visible. In either case, when you edit the feature you'll see all the dimensions, even to the non-geometry point. (The dimensions to either type will show up normally when in drawing mode.)

[jer3d1]

An axis will be created once the sketch has been used in an extrusion. Until then, the points remain points.

The axis available to sketcher is the construction axis which is on the sketch plane.

As for the help documentation, behavior like this existed in the past, perhaps it is out of date.


Jered

[rbutcher]

Nate,

See image below. The sketcher point option on the left, results in
creating a datum point (if only used in a sketch), or a datum axis (if the
sketched is used in an extrude feature). The sketcher point option on the
right is construction only and does not exist outside of the sketch.

Ryan Butcher

[rbutcher]

Nate,

Don't know if the image worked last time. I have attached it.

Ryan

[santinou]

I believe that area of creo help is referring sketched entities in drawing mode.

In Reply to Nathan Rollins:

Hi all,



I am trying to sketch a point and get a datum axis to show up. I found this
in the Creo help:







Do you see the "the entities appear on the model tree" ??? What is that? I
am missing something really obvious, right?



Sketched entities in the model tree? I have never seen that. Anyone out
there has?



Anyway - maybe you can tell me WHY I cannot get a sketched point to generate
a datum axis - like I have a thousand times before. Today it doesn't want
to work. I must not have my framis turned on or something.



-Nate

[mpeterson]

I am only familiar with this working when creating an extruded feature and you have to use the correct point in the sketch.Mark Peterson SentfrommyLGOptimusGPro™,anAT&T4GLTEsmartphone ------Original message------Fromanto UccelloDate:Mon, 6/16/2014 11:28AMTo-;Subject:[proecad] -RE:sketched datums
I believe that area of creo help is referring sketched entities in drawing mode.

In Reply to Nathan Rollins:Hi all,



I am trying to sketch a point and get a datum axis to show up. I found this
in the Creo help:







Do you see the "the entities appear on the model tree" ??? What is that? I
am missing something really obvious, right?



Sketched entities in the model tree? I have never seen that. Anyone out
there has?



Anyway - maybe you can tell me WHY I cannot get a sketched point to generate
a datum axis - like I have a thousand times before. Today it doesn't want
to work. I must not have my framis turned on or something.



-Nate


Site Links: View post onlineView mailing list onlineStart new thread via emailUnsubscribe from this mailing listManage your subscription


Use of this email content is governed by the terms of service at:

[JLG]

I thought this help was for Creo Direct (but not Creo Parametric).

Janet Grove

[nrollins]

Hmmm, I don't have Creo Direct..

[kimndave9]

The point->axis works in linear extrusions. I think it doesn't work in other extrustion; certainly not in revolves or sketched datum curves.

x

[mlocascio]

I am not really sure what Creo Direct looks like.



Michael P. Locascio

[mlocascio]

Typically IF you make a cylindrical feature it will have an axis. AND IF you
want to show an axis for a circular portion of a cut or extrusion you can
use the point/axis to definPe an axis.



Michael P. Locascio