more than one hole at a time

[locos]

I'm new here so i want to say hello everyone !
Thing is I'm advanced solid edge user and now i need to switch to pro-e. And i have one problem - using hole command can i create more than one hole at a time in pro-e ? this is how it looks in solid edge screenshot .One command was used and i can get as many holes as i want (with the same diameter of course)
If it's not possible how i can do this fast and easy? (btw i know patterns but I need different locations)
thanks in advance!

 

[miki12]

You can do similar as this through table driven pattern where you enter holes location dimension in relation from first hole created. You can even change a hole diameter of each hole or leave it the same.

 

[Bob_W]

Or, depending on depth, use extrude and create all the holes in one sketch.

 

[dgs]

Or, depending on depth, use extrude and create all the holes in one sketch.

This is the way I typically do it. Gives a lot of flexibility in dimensioning the pattern and aligning to existing geometry.

I thought in WF5 (Creo/Elements Pro) that you could create a sketch of datum points, and use those points to drive a pattern of holes. Best of both worlds.

 

[srieger]

I thought in WF5 (Creo/Elements Pro) that you could create a sketch of datum points, and use those points to drive a pattern of holes. Best of both worlds.

You have been able to do this for a very long time. Long before Wildfire.

 

[dgs]

I thought in WF5 (Creo/Elements Pro) that you could create a sketch of datum points, and use those points to drive a pattern of holes. Best of both worlds.

You have been able to do this for a very long time. Long before Wildfire.

Really? How? I'd love to do that.

To clarify, I'm talking about using sketcher to create several points in a single section (prior to WF5 this was a sketched datum point feature). Then, create a hole feature through one of the points. Then, pattern the hole by refference and get a hole at each point.

If I can do that now, man, I've been missing out.

 

[srieger]

Create a Sketchedpoint, pattern the sketched point by table (or other means), create a hole on the lead point, pattern by reference.


By doing it this way you can change the quantity of points/holes, dimensions, and use multiple pattern tables in a family table.

 

[troudt]

Create a sketch and place the geometry points(expand the point tool icon and select the second item) where needed.
Since the sketch is selected in the tree, start the hole command and it will automatically place the hole on the first point.
Finish the hole command and pattern it.
Change pattern type to point and select the sketch.
Exclude the dot on the first hole otherwise it will create and extra hole.

The nice thing about this is you can add and remove holes easily and in the mating part if you create the hole linking to the first point and pattern it will reference pattern.

I set these up as a udf and mapkey and can upload them if you want.

Using this and the hole config settings make the hole command quite useful now.

 

[dgs]

Create a Sketchedpoint, pattern the sketched point by table (or other means), create a hole on the lead point, pattern by reference.


By doing it this way you can change the quantity of points/holes, dimensions, and use multiple pattern tables in a family table.

Ah, but that's a different animal. Yes, that's always been possible, but even with a table driven pattern isn't as flexible as a sketch of datum points. Each point has to use the same dimension scheme and the same references.

What Troudt is saying is what I was talking about as being new in WF5. You don't pattern the point, you create a sketch, place many points in the one sketch, place a hole feature on the first point and then pattern the hole feature by reference and Pro/E will place a hole at each sketched point.

 

[jdurston]

I am a firm believer in patterning the axes or points and then ref patterning the holes especially in sheet metal parts, because, not only can you use this pattern in the assembly mode to ref pattern your hardware (screws etc.) and have that automatically update when the part pattern is modified, but also having the axis or point pattern allows more flexibility in changing the holes, to other types of punched holes (squares, hex punches or even knockouts). You could easily delete and create a new feature over the point or axis pattern leader and ref pattern again.* This preserves the original locations. Additionally, if you reference the original axis or point in the assembly mode, your fasteners wont fail upon regeneration.

You don't get this advantage with a extrusion with multiple closed sections generally. (Although, there are circumstances where it makes sense to use that technique.)

I believe a good modeler will prioritize how the model will behave in modification vs. speed of creation. Think about the next guy who needs to make a change to your model.

* - In many cases, changing the sketch built around a singular point reference is easy to do as well. There are no worries on messing up the feature locations this way.

 

[srieger]

@dgs


I see, but if you are using different references then it may not be best to use the same pattern. The more complex you make a feature like this the less robust the model is. Part of proper modelling techniques is to simplify features in order to make the model optimally flexible.


I know, "proper modelling technique" is subjective. Yes, it may be easier and quicker. To me, this would not be the best way to do it.Once you have multiple references, you run double the risk of failure should modifications change in such a way as to eliminate one of the references. Then all the holes would fail.


If you need to have multiple references, then in my opinion, you need to have multiple patterns and pattern tables. Then, if one of the features is modified to a point that it affects the reference, only one set of holes would be affected.

 

[aaronk]

Create a sketch and place the geometry points(expand the point tool icon and select the second item) where needed.
Since the sketch is selected in the tree, start the hole command and it will automatically place the hole on the first point.
Finish the hole command and pattern it.
Change pattern type to point and select the sketch.
Exclude the dot on the first hole otherwise it will create and extra hole.

The nice thing about this is you can add and remove holes easily and in the mating part if you create the hole linking to the first point and pattern it will reference pattern.

I set these up as a udf and mapkey and can upload them if you want.

Using this and the hole config settings make the hole command quite useful now.

THANK YOU, THANK YOU, THANK YOU! I knew there had to be a way to do this. I even called PTC Tech Support, but they couldn't help me. This is perfect for putting in hundred of ejector pin holes! (usually not a simple pattern)