Centre lines???

[ptc-4339982]

Having only had Creo for a couple of months I have yet to do any serious detailing until now.

I have not yet found a way of showing centre lines on my drawings. I have heard that it is not possible simply add centre lines to a 2D layout which makes detailing ducting inparticular a serious headache, is this the case and if so are there any work arounds which you can suggest?

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.

[KevinBradberry]

You can quickly make a centerline wherever you have axes in your model. Use Show Model Annotations to choose axes for centerline creation. Select the tab to the far right.

Extra info:

Creo automatically creates axes in your solid model when you extrude circles or make holes, but if you wish to have axes created any time your extrusion contains an arc set the option show_axes_for_extr_arcs to yes. I don't think there is a way to have axes automatically created when you create a Round feature.

Also helpful, you can erase, not delete, one of the lines of the crosshairs by highlighting it, right-clicking and selecting Erase.

My question:

Does anyone know a workaround for resizing the centerlines shown in the image above. No matter which end you select and drag to extend the axis, all 4 ends will extend together. I want to be able to extend each one individually. I don't remember this being an issue before I used WF5.

[GrahameWard]

You're right, I hadn't noticed that before. Another thing I did notice is, if your axis is in side view, i.e. a single line instead of a cross hair, I find I can't stretch it beyond a certain point. It kind of somersaults over its opposite endpoint. IOW it is limited to the geometry of the feature it comes from.

[KshetrabasiMaha]

Hi Grahame

Try to pull the axis line in side view with alt button

You will be able to resize it easily

Regards

K.Mahanta

[KevinBradberry]

Kshetrabasi,

Thank you, that worked!

[ptc-1949899]

Re: My question,

You select the cross hair then grab the handle at the end of axis segment that you want to extend (your pointer will change to a single axis arrow when you hover over the handle) then stretch it out as far as you need. If this is what you are already doing, then I am not sure what the problem is, as this has worked on every version of Pro E. and Creo that I have used. If you stretch out the centre lines with the two axis arrow, all four segments will become the same length and move with the cursor. This is a pain if you have already spent time adjusting three segments and slip when clicking to adjusting the fourth. Incidentaly, if you like to have your drawings absolutly perfect, the handles at the end of any centre line will snap to the same snap lines as dimensions do.

Nice tip reagarding the erasing of single segments. Thanks for sharing.

[KshetrabasiMaha]

Hi Kevin

This option was modified slightly

If you want to extend only one side of the 4lines of the axis; then you have to try this with alt button

Press alt button and drag

Regards

K.Mahanta

[AmitDeshpande]

Hi Steve,

If one of the responses helped resolve your issue, would you please mark it as the Correct Answer?  That way other users visiting the discussion will know; as the correct answer gets copied right below the question.

Thanks,

Amit