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Why must I

M

michaelpaul

New member
measure a radius one way and a diameter another way (sometimes) in the model?

I know that there is an Info - Measure - diameter option but that doesn't seem to work well on a drafted cylinder. it gives me a diameter measure but not necessarily the one I want to measure.

So that means I must then go to Info - Geometry - Radius to select the actual edge I want to measure. Then, I must open Calculator and multiply that value by two in order to determine the diameter.

Kind of a pain in the you know what...........

Back in SW, you pick the edge, you click the measure tool and presto, the diameter is displayed. pretty darn simple..................

Michael
 
Michael,


Try Info>- Measure>- Curve Length


Kev


EDIT


Personally I have a load of mapkeys (could also be a menu if you like) that I use to do all my measuring, which means that I am dreading moving to WF3, coz as far as I can see it has all gone to s*%t there


Kev
Edited by: prohammy
 
smiley36.gif
 
Measure Diameter only works for surfaces and a Tapered Cylinder doesn't have a Diameter value.

The Radius Measure Will give you major and minor radii at any point.

The best method is to just create a dimension in your model using the following procedure.

Applications > Legacy > Setup > Dimension
Select the plane for dimension to be parallel to any plane parallel to the edge you want to measure the diameter of.
Select the arrow to face the direction you want to read the dimension from.
Hit Okay
Double click the edge and hit middle button to place and you'll get a 3d Dim from the cylinder edge.

View attachment 4325

Once the Measurement Dimension is made you'll have easy access to it any time from the Model tree by Displaying Annotations.
Go to Tree > Item Display and check box for Annotations and you'll see default dimension names ad##, ad## .
You can change these by right clicking and selecting Properties the Dimension Text tab and enter the symbol you want in the Name box and hit OK.
Then whenever you want to see the value Right click the Annotation Name you want and select Value and you'll see the value display on Screen in Huge Red Text. The red below is from model tree highlight the Value Red is much bigger.

View attachment 4326
To hide the dimension/s you can put it on a layer by creating a layer like 00_Diameter_Meas and adding it to that layer by going to Layer Properties and choosing Dimension as selection type and picking it on screen.

If the Layer is hidden the Value option will no longer be available in the model tree but you can select the name in the Layer Tree and it will show on screen.

If you select Properties it will become unhidden and only re-hide after a change is made in Layer Visibility. This is a Bug so I suggest selecting the dim from your layer items to see it display.

If you don't want the dimension to show you can go to text style and make it really small. Then Select the Dim and Choose Value from the model tree. when you want to see the value.

Michael


Edited by: mjcole_ptc
 
I'm with michaelpaul; why it got to be so d*mn hard!! SW you can measure diameter, radius, plane to plane, edge to plane, and any of the combinations all with the same function!! PTC WAKE UP!!!!!
smiley7.gif
 
To add the dimension as I described is not at all hard and you don't have to select measure all the time.

You can use Measure distance and pick opposing vertices on the cylinder and get your Diameter. Also how hard is multiplying by 2?

I'm just very descriptive with my answers and gave more than was necessary for my answer.
 
prohammy said:
have a load of mapkeys (could also be a menu if you like) that I use to do all my measuring, which means that I am dreading moving to WF3, coz as far as I can see it has all gone to s*%t there
Click to expand...


Many thanks to Michael for that tip. One more question thought. What exactly did you mean by this Prohammy. The reason I ask is because I am on WF2.0, and will later move to WF3.0...Are all of my mapkeys not going to work or aomething?


Omar
Edited by: omarhernandez
 
mjcole_ptc said:
The best method is to just create a dimension in your model using the following procedure.
Michael
Click to expand...

Michael,

thanks for the tips. I'll look into doing this but.............

it's far from straightforward to do it this way. Usually, I just want to know what a diameter is on one part, so that I may create a corresponding feature on a mating part with clearance. So, generally I only need to determine the diameter one time. this goes back to my original comment that while the information can be obtained, it's not necessarily easy or intuitive to get it from ProE.

Michael
 
jelston said:
I'm with michaelpaul; why it got to be so d*mn hard!! SW you can measure diameter, radius, plane to plane, edge to plane, and any of the combinations all with the same function!! PTC WAKE UP!!!!!
smiley7.gif
Click to expand...

I REALLY miss the ability in SW that it would give you the X-Y-Z distances as well as straight line distance all at once when you measure. Pro, nope. pick your points, then change your projection reference to Csys, pick your csys, hit calculate, zoom out to find where your X-Y-Z are and then figure out which direction you want to determine. Arghhhhhhh!

Michael
 
Michael,

You can get the XYZ in addition to straight line measurement in Pro/E by selecting CSYS as measurement type like you said. But a good thing to do after going through the trouble of setting up this Analysis Measurement using CSYS is to save the Analysis so you can retrieve it and only have to select references and not the CSYS.

Saving Specific Measurement Types
<br style="color: rgb(0, 0, 255);">To determine which direction X,Yand Z are without zooming to see the CSYS you can look at the spin center. I've copied the default CSYS into the image in the above link and describe which color refers to which direction below.
A good way to tell which direction of the CSYS you want to find without having to Zoom out is to lok at the Spin Center's Red Graan and Blue knobs. These always point in the same direction. In the Default Pro/E set up where the X and Y are along the Front Plane the
Red Spin Center knob is X direction
Green Spin Axis Points in Y direction and the
Blue Spin Axis points in Z direction Normal to the front plane.

Red Green Blue = X Y Z

I showed a co-worker this once and he was glad with knowing how to retrieve analysis setup. Hope this helps you.

Solid works does do measurements a lot nicer and allows center to center distance with out selecting Axes. I mean you can do center to center dims why not allow Center point as a selection type.

View the evidence PTC shows dx dy dz on the same line WTF?

View attachment 4327

I understand where and what you are coming from.

Michael



Edited by: mjcole_ptc
 
Prohammy, Omarhernandez,


Unfortunately i have just moved to wf3 and yep the measure function is a ptc upgrade, it seems to require more mouse clicks than before. Strange that!


I use a spaceexplorer and used to be able to click one button and up came the dialogue box, ready to measure. Just had to change the measurement type (curve length, distance etc). Now all it does is expand the analysis drop down menu, which i could have done with one mouse click. I don't use mapkeys yet so i don't know if they will work or not. Keep your fingers crossed.


Mark
 
Omar,


Had a chance to 'play' with WF3 and honestly the changes they have made to the measure tool are awful.......Cheers to PTC for adding another feather to the SW bow


Kev
 
As mjcole_ptc has once again pointed out, the 'Easy' button has been overlooked by PTC. Function settings that should be the default requires an extensive knowledge of the royal hieroglyphics in Pro/E. It just amazes me that PTC can't figure out the simple stuff after all these years. I guess NIHhas beenthe order of the day at PTC for many years.
 
Easier Button Method,

It is actually possible to measure what you want with the Diameter measure option even though it requires you to pick a surface to measure first.

If you select a point to measure at, which is allowed but not required by the Definition Dialog Box, you can select a point on a surface edge where you want the measurement made and you don't need to make a dimension like the previous technique I outlined. This is possible many ways but the easiest way to have it give you the value where you want is to set your selection filter to Edge Location as shown below.

View attachment 4330

This method also shows you visual note for the measurement which you
can show or hide from the Saved analysis dialog by clicking on the
(EYE)con next to the name.

View attachment 4331

You can access the Saved analyses or Hide all at any time Using the Icons or Analysis > Saved AnalysisAnalysis > Hide All

PTC has had this functionality since way back and have never bothered to change it. They just mapped new paths to accessing it much like Windows still uses old DOS functionality even on it's latest systems. Eventually when enough customers leave them they'll get the idea.

In WF3 the only update is new icons which I already have for my mapkeys so it is a bit simpler but there is no actual change in the functionality of the measurement programming.

That is some well spent time I'm not even going to calculate the pixels created per week value on that one. Maybe they can add a Time Wasted analysis measurement when they decide to update the user interface.

It's a shame that in this Area where Object Action would be useful as in Selecting an Edge and being able to Right Click and select Get Entity Info hasn't been created as a functionality.

Michael



Edited by: mjcole_ptc
 
This is one area where ProE sucks. For a new user, it is so difficult to take a measurement and be sure that the answer that you are being given by ProE is the one you are after. MJCOLE has shown a number of ways to measure (thanks for that) but it shouldn't be that difficult.


PTC, why do you make things so difficult??????????
smiley7.gif



If the group I work for hadn't hired a PTC person who is driving every group to move to ProE, I would urge them to change to SolidWorks. Less time would be wasted on taks that should be a lot more intuitive.


Michael
 
michael3130 said:
Less time would be wasted on taks that should be a lot more intuitive.
Click to expand...


I totally agree! The biggest problem I face on most days involves Pro/E and not the products i design!


I have installed and setup both SW and Pro. With SW, i hit the ground running after installation, with Pro, I have to find a buncha freakin options! SW comes preconfigured for ANSI or ISO and others. WAKE UP PTC!!!
 
Has anyone ever had a problem with the mearsure dialog box showing insufficient number of decimal places. Sometimes it shows me 6 and other times is only shows me 4. Then I check in sketch and I actually have more than i was shown in the dialog (measure) box. Has anyone ever hadthis probelm?


Omar
 
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