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Show Centre Mark for groove on OD

K

Khobin

New member
Hi,


I have a revovled surface that has a radiused groove on it, see screenshot below. The feature is dimensioned to the centre of the radius, and the dimension shows up fine on the drawing, however, for clarity I would perfer to show the centremark on the drawing as well.


From searching online it seems the best way to create a datum axis in the model and show it, however, because the centremark I want to show isn't on the surface of the model, I can't seem to get a get a centreline to pass through it. I've also trying making a datum point, the problem with it is that it doesn't come through using the show/erase tool, and if you just make datum points visble it can be seen in the drawing, but is at a bad scaling and has a tag on it, and just creates clutter instead of being useful.


Is the only viable option to create a clean centremark in Pro-E to use the (terrible) sketcher in the drawing itself?


View attachment 5236
Edited by: Khobin
 
You might want to offset a datum from the center of the revolved part to the center of the radius, then just usethat datum and a vertical one thru the radiusto create and axis (making sure its in the same view thats on the drawing). You can use relations to keep it all parametric.


Its clumsy but off the top of my head thats all i can think of!


Garymig
 
You can also create a curve from the intersection of the groove surface and a plane and place an axis through the center of the arc that is created.
 
Thanks for the suggestions.


Ihave 4 of these grooves on 1 part, so that's an extra 8 features just to be able to put a centermark on a drawing, lol...
 
Not that it's a big deal but if you use the intersect method you could do it in five since the groove surfaces can be included in one intersect feature.
 
@kdem


Thanks for the tip, I'll try that sometime when I have time, got side-tracked with another project for now.


@dr_gallup


For the same reason you typically dimensionholes to the centre... Dimensioning to the centrepointis often much more helpful for machinists/cnc programming. For inspection you are correct, it's hard tomeasure a point that'sout in space.
 
After creating your revolved part, you can create a secondary sketch that uses the revolved surface as a reference. You can draw a circle in the sketch and use that to create a center. Hide the sketch and the center line isparameteric to the groove in the part. This requires onlytwo features.
 
Hi mstout.

I'm very curious about your method but I don't understand what you mean by "create a center". I tried what you said, created a circle in a separate sketch, but could not get an axis out of it. Could you clarify this?

Thank you,
 
Khobin, all you need to do is create a singleaxis feature. Make it normal to the plane you sketched your revolved section on and make it reference the same reference datums as your revolved sketch, usingdimensions.


If you want the axis to be parametric to the groove use relations.


View attachment 5290
 
hmm, I see a few issues with that:
- extra axes that aren't "actual" axes clutter up parts that already have too much going on when you show axes/planes.
- what if you have a part with 20 of those grooves?
- relations! relations should only be necessary if you plan on doing some sort of math, IMO. simply referencing other features should be a part of your basic modeling tools.

Not to say it isn't the best solution yet, it is only 1 feature... per groove.

But really, this should be done in 0 features. If you draw a curve with a centre point in a sketch, why can't you show that centre in the drawing? This is elementary stuff.
 
An axis is represented when a feature has an axis. Adding one may more more confusing in my opinion as in this case the feature doesn't have an axis at this position. The only axis would be at the center of revolution.


You refered to a hole as something similar, but a hole actually has an axis.


Personally, I think you may be over thinking it. Sometimes when a detailer adds something while attempting to add clarity, it causes more clutter and confusion. Stick to the basics and the standards and everyone should understand.


Dimension to the center if this is how you wish to control the part. I don't believe there is really a need to add a center point.
 
srieger,

What you are saying is that dimensioning groove depth, groove radius, and distance from end to centre of groove (well, the machinist has to assume it's the centre, as there is no centre mark) is a better way to dimension than marking a centre then dimensioning the position of the centre and the radius/diameter. I would say it's a preference and that the designer should be given the choice on how to dimension it.

We work in a predominantly AutoCAD office that is slowly moving to Pro/E. Restrictions on choice such as this sure don't make it easy to convince others to switch to 3D.

I agree there should only be an axis if a feature actually has an axis... that's why I'm saying Pro/E should give the choice to place a centre mark at the centre of circular features
 
Yes, it's dumb that ProE doesn't let you add an axis to a toroidal groove. If you want to do a pos-tol you would dimension to the CL of the sketched groove radius with boxed dims. Personally, I think it's an oversight by PTC.


The toroidal groove does have an axis. It has a 360deg curved axis. At any given point thataxis ought toshow up on a drawing view as a tangential axis. It's a shame it doesn't.


You can create the axis as I said above with a separate axis feature, or as a previous poster said by extending and breaking the witness lines. That's the method to use if you dont want additional axes cluttering your model.


ALTERNATIVE METHOD


Create ashort straight holethe size and position of the toroidal groove. Then createyour revolved toroidal section using the hole to drive all the dimensions. This way, although it's still an extra feature the toroidal groove will cut through the hole so it's not visible in the model, there are no extra dimensions, and you can show the hole axis on the drawing. You can pos-tol the dimensions of the hole easily.
Edited by: dakeb1
 
You can placea center mark in the drawing itself by creating a point that is constrained to the center of the groove arc. Just be sure to associate it to the view or it will notmove with the view. You will also need tofix it should you change the scale of the view.
 
dakeb1 said:
The toroidal groove does have an axis. It has a 360deg curved axis. At any given point thataxis ought toshow up on a drawing view as a tangential axis. It's a shame it doesn't.
Click to expand...


An "axis" is linear by definition and cannot be defined here. It would not be an oversight as what is being asked to be done here is not defined by any standards (ie. ISO, ANSI, DIN, JIS, etc). PTC sticks to the standards.


This is why I recommend sticking as close as possible to the standards. Everyone is on the same page as long as they have a standard for interpretingthe drawings. Once you start making stuff up as you go, the interpretation becomes questionable. How do you interpret a drawing that is outside the scope of a standard... You can only make assumptions. This is what leads to trouble.
 
srieger said:
dakeb1 said:
The toroidal groove does have an axis. It has a 360deg curved axis. At any given point thataxis ought toshow up on a drawing view as a tangential axis. It's a shame it doesn't.
Click to expand...


An "axis" is linear by definition and cannot be defined here. It would not be an oversight as what is being asked to be done here is not defined by any standards (ie. ISO, ANSI, DIN, JIS, etc). PTC sticks to the standards.


This is why I recommend sticking as close as possible to the standards. Everyone is on the same page as long as they have a standard for interpretingthe drawings. Once you start making stuff up as you go, the interpretation becomes questionable. How do you interpret a drawing that is outside the scope of a standard... You can only make assumptions. This is what leads to trouble.
Click to expand...


By "curved axis" I mean trajectory.


It's all very well sticking to standards, but in the case of a toroidal groove machined on a diameter there is no standard defined for dimensioning it, so in this case we have to make it up as we go along.


With that in mind it is sensible to dimension the sketch that generates the torioid, as the sketch is basically an arc drawn on a flat plane. It is the arc of this sketch that has an axis, albiet a 2D one. The OPwants to show the 2D axis of this sketched arc, in a drawing whose view is in the same planeas the sketch.


Ignoring the revolved toroid,my argument is ProE does not even allow you to show the 2D axis of the sketched arc, and that IS within the scope of the standards. We don't need ProE to show a tangential axis, but it seems to be the only way to produce a 2D axis in a drawing view (without sketching it of course, which is tedious and not parametric).
 
snufflufikist said:
Hi mstout.

I'm very curious about your method but I don't understand what you mean by "create a center". I tried what you said, created a circle in a separate sketch, but could not get an axis out of it. Could you clarify this?

Thank you,
Click to expand...


After you have created your model, youmake a secondary sketch that is on the same sketch plane as the revolve sketch. The seconday sketch would contain onlya circle in it that is referenced to the revolved circle. This establishes its location and size. Then exit the sketch and start theDatum Axis Tool to add a centerline. Use the secondary sketch circle as the reference for the centerline. This method will ensure that the centerline is in the correct place even if the size or location of the feature is changed.
Edited by: mstout
 
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