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how to show or draw center mark

ptc-1647943
1-Newbie

how to show or draw center mark

I realize that the show/erase just can show the axis of round feature object, but it can not show the centerline/mark of revolved feature with radius. For dimensioning purpose, I do need centermark as references. Any idea to solve this simple issue? Thanks in advance, Yong
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1 ACCEPTED SOLUTION

Accepted Solutions
cgorni
15-Moonstone
(To:ptc-1647943)

To close this community thread on the ability to show Center mark for Rounds or Arcs in the drawing.

 

Summary of the proposed solutions:

 

  • For extruded features:
    • You can set the configuration option show_axes_for_extr_arcs to yes, then axis will be automatically added when creating new Extruded features, for example for all fillets in the Sketch.  See article CS77534
    • If you prefer to only have axis for individual items and arcs you can instead use Geometry Points in the Sketch to specify where the axis will be added, see article CS37345. Please refer to article CS171458 for more details on hiding those axis with layers when working with quilts.
    • Datum Axis can also be created afterwards from the Model tab of the Creo ribbon picking the extruded cylindrical surface.
    • All those Model datums can then be shown from Annotate > Show Model Annotations dialog in the drawing

 

  • For revolved features:
    • Above solutions are not available and an additional Sketch can be used to insert Datum Points and then create Datum Axis, anticipating their location in drawing views

cgorni_0-1634820937914.jpeg

 

Then Show Model Annotations dialog can be used to display center marks in 2D:

 

cgorni_1-1634820937918.jpeg

 

  • Alternate 2D methods:
    • Directly sketch entities in the drawing and modify their line style to mimic centerlines, see CS265771

This Product Idea was previously filed to request an enhancement in a future Creo releases and archived, new ideas can be submitted in the dedicated section.

View solution in original post

24 REPLIES 24
SkyKing
5-Regular Member
(To:ptc-1647943)

Creats points on drawing or Datum Axis on model.

My method, In the drawing, dimension the radius to it's center point. Then click on the dimension and hold down the rt. mouse button to display the shortcut menu, select "clip witness lines", pick the dimension and the dimension line (turns green), extend the line thru the radius origin. Next select "insert" break and break the witness line to create your horiz. & vert. origin lines. When finished, you can select the dimensions and adjust the break as needed.

Yong, I'm not sure what your problem is in Drawing mode. If you are creating a dimension, pick Center from the ATTACH TYPE menu displayed in the upper right. This should work for all types of geometry, not just holes. However, following on the response of Sokheng Chheng, it is a good idea generally to anticipate the downstream need for axes while creating features. (1) Axes of revolved features can be created as you make them. (2) Axes of extruded surfaces, even edge rounds, can be created after the fact by selecting the Create Axis icon and the "revolved' surface. (3) For extruded features, the axis can be created ahead of time (while sketching) by selecting Axis Point from the Sketch drop-down list, IF the sketch is an Internal Sketch started after the Protrusion is started. David

Zong, I think you're trying to make something like, e.g. an elongated hole feature that has two default center/axis. Show/Erase will not auto-show unless you apply the method (3) in David's post. It works very well. I do that all the time so I don't need to create redundant datum axis in the model tree.

"Tan Le" wrote:

Zong,

yes we can get the axis on the arcs which we create in sketcher with a config.pro option show_axes_for_extr_arcs yes try this i beleive it can help you but this dont add axis in rounds it can only create the axis wen sketch section contains arcs

I really appreciate all the wonderful helps from you guys. Yong

Tan.Le---Using the datum axis or point only works in the extrude feature. Does not help with a revolve feature.

Sokheng---Adding a point to the drawing puts an X on the drawing for the centermark, not a true + sign.

Troy

Is there a way then to put a centermark on that circle/slot center etc.? I know how to dimension to the center, but if you don't put a centermark, then it looks as though your dimensioning to a random spot on the drawing. I don't want to have to add anything to the model and then show it in the drawing (then make sure all other axis or whatever are hidden), because frankly, that is silly and cumbersome. Centermarks and centerlines are basic 2d drawing standards that should be easy to show. In other programs there would be an icon called centerpoint or centermark that you would just click the circle, arc etc and it would create a centermark. Am I missing something, or is ProE just made to be cumbersome?

I believe what you want is to create an Axis Point while in the Sketch of the slot. This will show up as an end-on axis in your drawing, i.e a "center mark".

In the case of an obround slot (one of the commonest uses for this), just put a centerline through one of the arc centers parallel to the slot extent, and another perpendicular centerline through the midpoint of the straight side, and an Axis Point at their intersection.

It's impressive how complicated is a simple thing, like to put a center mark, in Creo can be so much complicated. In Autocad, Inventor and solidworks is just a simple button...

If anyone can make a tutorial to make a center mark in the drawing without doing it by "hand" please let me know. I will apreciate.

Thanks and best regards

Nuno

Assuming you are trying to dimension to the centre of an obround, this is the easiest way I have found:

Open the Sketch of the obround feature for editing. Draw a diagonal line from one end of one of the straight lines of the obround to the opposite end of the other straight line. RMB, Convert to Construction. Sketch, Axis Point at the Midpoint of the construction line you just drew.

Now, when you show the axes of the obround feature in the drawing, there will be one at the centre of each radius and one in the middle of the whole thing.

I hope this makes sense. If not, feel free to ask.

John

Here is what I found. Under the "Annotate" tab, select "Show Model Annotations" and a dialog box should appear. Select the right most tab on the box titled, "Show the model datums". Click the feature you want a center mark for, and then click the check-box tab in the dialog box; this will add your center mark.

While we're on the subject, you can also turn on the option to have extrusions with less than full rounds generate an axis.

config.pro - show_axes_for_extr_arcs yes

If you are a minimalist, you won't like it, but if you need it, it can be created by default.

We want to dimension from the end face to the centermarks of the radii in this item, in order to show where the arc center is located. How do we show them? This is a revolved feature creating this cylindrical part.

Troy

centermark.jpg

Is this in the model or in the drawing?

If it is in the drawing, you can shown annotation and have the centerline of the cylinder (right side) or the center mark of the endviews (left) show up as selected.

As shown below, A_1 is selected and shown up in yellow. The rest in red haven't by selected. Then either hit apply or OK.

Thanks, Dale

centerlines.jpg

Capture.PNG

Dale, this is the result of a work around that I was creating, but found out the hard way if someone responds to your post, it is no longer editable??>. LOL

These results can be accomplished by creating a seperate sketch on the viewing plane, using Project on the sketching tab, referencing the radii, then adding vertical DATUM centerlines to each centerpoint, and add horizontal DATUM centerlines to EACH centermark (these will overlap here), then accept the sketch, return to drawing, and Show Model Annotations to show all axis/datum lines for the features. You may now use the grips on each centerline to adjust the sizes of the datum lines. If necessary, you may make your view INDEPENDENT from the drawing and hide the sketches; it will leave the "centermarks" alone.

Troy

From the revolve itself, there should be an axis that you could show through the annotations both the longitudinal axis and the centermarks on the end view.

This is an unusual case for requiring the center cross-hair. You can either sketch them (high pain level) or you can add geometry point in the revolve sketch. You can define a datum axis through the geometry point. You have to know that your orientation of the sketch will coincide with the drawing as expected. There is no clean way to do this until PTC sees that having optional center cross-hairs should be part of the dimension leaders, not just axes.

SkyKing
5-Regular Member
(To:ptc-5114571)

Untitled.jpg

Use sketch to make points. Use those points to make axises. On the drawing, use show model annotations to show axises (centermarks).Untitled1.jpg

SkyKing
5-Regular Member
(To:SkyKing)

Untitled.jpg

above can less some steps

centermark command like autocad would be nice also

cgorni
15-Moonstone
(To:ptc-1647943)

To close this community thread on the ability to show Center mark for Rounds or Arcs in the drawing.

 

Summary of the proposed solutions:

 

  • For extruded features:
    • You can set the configuration option show_axes_for_extr_arcs to yes, then axis will be automatically added when creating new Extruded features, for example for all fillets in the Sketch.  See article CS77534
    • If you prefer to only have axis for individual items and arcs you can instead use Geometry Points in the Sketch to specify where the axis will be added, see article CS37345. Please refer to article CS171458 for more details on hiding those axis with layers when working with quilts.
    • Datum Axis can also be created afterwards from the Model tab of the Creo ribbon picking the extruded cylindrical surface.
    • All those Model datums can then be shown from Annotate > Show Model Annotations dialog in the drawing

 

  • For revolved features:
    • Above solutions are not available and an additional Sketch can be used to insert Datum Points and then create Datum Axis, anticipating their location in drawing views

cgorni_0-1634820937914.jpeg

 

Then Show Model Annotations dialog can be used to display center marks in 2D:

 

cgorni_1-1634820937918.jpeg

 

  • Alternate 2D methods:
    • Directly sketch entities in the drawing and modify their line style to mimic centerlines, see CS265771

This Product Idea was previously filed to request an enhancement in a future Creo releases and archived, new ideas can be submitted in the dedicated section.

View solution in original post

StephenWilliams
22-Sapphire III
(To:cgorni)

@cgorni  The product Idea linked to is "Archived" so by definition;

  • Archived:  This idea either did not get the necessary support of other community members in the idea submission time frame (varies by segment),  or was a “legacy idea” that was not included in the new 2019 Community Ideas Program.  Re-submission of ideas is an option for relevant product enhancement requests.

https://community.ptc.com/t5/Welcome-How-To-s/PTC-Community-Idea-Status-Definitions/m-p/607213

 

@StephenWilliams , you're right.

 

Sorry for the confusion, I edited the post.

 

Thanks for the notice.

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