What is in the cards...
* What is a DIM BOUND and its use?
* How do I access it?
* What are my options?
* Maximum Material Condition (MMC) and Least Material Condition (LMC)
* Dim Bound TABLE
What is a DIM BOUND and its use?
We will have a look at the possibilities of using the ProE option "DIM BOUND". With this option you can set the model dimensions on its tolerance limits and the model will get changed to that limit, without manually modifying the value. Thus, you can have a model, that is on a tolerance limit. This is useful in tolerance stack-up analysis or worst case analysis.
For Eg, if you have a dimension "50 (+5 / -2)" and set it to its upper limit using this option and measure the length, you will get 55. But the Dimension Value remains the same as 50 and the model gets modified to its limit value (55). We will have a close look at it now.
How do I access it?
Here is the command
Edit menu -> Setup -> Dim Bound.
What are my options?
Options on limit
With this option, you can set single (or multiple or all) dimension(s) to the following possibilities.
* UPPER Tolerance Limit
* LOWER Tolerance Limit
* NOMINAL
* MIDDLE of the Tolerance Limits
Note: if you have not set the tolerance, it will take the default tolerance.
Options on dim selection
A) You can set all the dimensions to any of the four choices.
B) You can set a selected list of dimensions to any of the four choices.
C) You can use "DIM BND TABLE"
Options A and B are pretty straight forward. Select the option - Select one or more dimensions and say OK/Done. Model would have got changed.
The Option C (DIM BND TABLE) allows you to save, retrieve and edit (in a table) the setting that you want. We will see this later in the post.
Maximum Material Condition (MMC) and Least Material Condition (LMC)
On a simplistic level MMC and LMC are achieved as....
MMC => Maximum Diameter of shaft and minimum diameter of hole.
LMC => Minimum Diameter of shaft and maximum diameter of hole.
If the increase in dimension increases the material, then for MMC it should be on UPPER limit and for LMC it should be on its LOWER Limit. vise versa.
For "Maximum Material Condition" (MMC) and "Least material Condition" (LMC), you have to set the dim limits manually. ProE, as far as I know, does not have the functionality to automatically identify the dim limits for MMC or LMC condition. Hence what you have to do is to identify yourself the dimensions that are to be set at its UPPER limit and that are to be set on LOWER limits in order to simulate the MMC or LMC. On a simple logic, for an MMC, all external dims should be on UPPER and all internal dims should be on LOWER limits. vice versa for LMC.
DIM BND TABLE
The "DIM BND TABLE" is very useful if you have to repeat certain tolerance bounded conditions. Assume you have 20 dimensions that you need to set on MMC and LMC. Using Dim Table, you can define the limits of each dimension in a table and you can use that to set the model to a certain state.
As you can see there are few options for DIM BND TABLE.
* You can save the current configuration with name.
* you can Apply a set thats previously saved.
* You can go into the table and edit the configuration.
In edit mode, you have each dimension as a column and each set as a row. comments are there at the top of the Edit window which is descriptive enough.
So don't forget to DIM BOUND the dimension(s) when you need to set the model on its limits.
Pro/E - Sketcher - Intend Manager
The Intent Manager enables you to dynamically dimension and constrain geometry as you sketch, which makes us to sketch very quickly. This auto recognizing tool is new option only available in proe wildfire versions. If you want to work in old menu manager environment switch off intend manager
(Sketch menu > unselect Intend Manager).
Intend manager creates weak dimensions and recognizes all possible constrains / Relations while you are drawing. To set the options for Intend manager auto-recognition of constrains go to Sketch > Options > Constraints. Select the constraints you want auto recognize. By default all constraints are being selected.
And then while sketching, you can temporarily switch off and lock constraints.
For example, draw one circle. One second, draw second circle. While, creating second circle, after specifying center point, move cursor away from center point to specify approximate size. Now, at some equal position proe highlights equal radius relation in red color (R1-for equal radius). Similarly, if you have line, when creating new line, at some equal distance, proe displays equal length (L1, L2... like this – for equal length relation). At that time, you can deactivate the relation creation just by clicking right button. Now specify second point for line, circle.
You can also lock the relations if you want keep them permanently by Shift + Right click, when proe highlighting relations in red color
Advanced Geometry- Unlocking the Potential of Pro/ENGINEER
Introduction
In this tutorial you'll learn some helpful tricks and methods to improve your design techniques and modeling skills using Pro/ENGINEER.
We'll cover Advanced Geometry topics ranging from variable section sweeps to advanced patterns and warp features.
1. Variable Section Sweeps
2. Patterns
Pattern Table
Fill Pattern
3. Warp Feature
4. Surface Operations
Surface Replace
Surface Solidify
What are the general methods of selecting surfaces?
The main classification of surface selection is..
> Individual Surfaces
> Bounded set
> > Neighbouring surfaces
> > Surface between anchor and boundary (or seed-boundary)
> > All surfaces
> Exclude surfaces
Before going into the main topic, we just have a look at other options.
Individual surfaces : Select all necessary surfaces one-by-one.
Bounded Set -> Neighbouring surfaces : ProE selects all neighbouring surfaces of the anchor surface.
Exclude Surfaces : Individually select surfaces that has to be removed from the selected ones.
What is seed-boundary surface set?
In this option the user selects one surface as anchor (the seed) and one (or more) surface(s) as boundary surface(s). ProE then takes all surfaces starting from anchor (seed) and bounded by the boundary surfaces.
How do I do it?
(Option-1)
Assume you want to make a copy of a surface set by this option.
Step 1:
Select the surface which will be the seed. In part level, if the selection filter is "SMART" then first click will select the feature and next click will select the geometry (surface, edge..). Or else you can change the filter to "GEOMETRY" and then select the surface easily.
Step 2: Edit-Copy (Ctrl+C)
Step 3: Edit-Paste (Ctrl+V)
At this stage it will look something like this.
Step 4:
Click "Details" and Click "Add".
Now select the anchor and boundaries.
Then it should be looking like this.
Step 5:
Click OK and your surface is ready.
In case you see one more entry here (single surface), right click and remove.
(Option-2)
I prefer this one, as this is easy!
Step 1:
Select the Seed surface.
Step 2:
Click SHIFT Key.
Step 3:
Select the boundary surface(s).
Step 4:
release the SHIFT key and the ProE will display the the surface set.
Now you can rotate the model.
Again you click SHIFT and continue the boundary selection. Releasing the SHIFT will update the surface selection.
Note:
You can do the Ctrl+C Ctrl+V to create a copy of this surface set.
Steps 1 to 4 can be followed in other surface selection situations. Like, you wanna apply the colour to all the surfaces in a pocket. Its easy with this as you don't have to go and select all surfaces one-by-one.
But the real power of this some things else.
What are the advantages?
When you make a pattern of a group of features, this comes really handy. In fact this is better than the feature pattern in terms of performance also.
Consider the model that I showed above and I wanna pattern the pocket.
Normal options are
1. make a group of the Cut-Extrude and the Round. Pattern it.
2. Make a pattern of the Cut-Extrude. Make a Ref pattern of the Round.
Here I will make a surface copy (selected with seed-boundary option) and make a pattern of it. Then make a soldification of the surface and make a reference pattern.
Now I want to change the pocket. I not only want to change the dimensions, I want to add some features in the pocket.
You just have to go to the inset mode above the copy feature, add your features and remove the insert mode. See what happened! The new features are updated in all pattern elements.
This option is so very useful in ProE when you have to deal with complex geometries and features. This is more important because if you do a GROUP and pattern, its almost impossible in ProE to add or remove some features from that. By this option these hassles are more or less avoided.
Have a look at the model tree. I just added the three features in between and the pattern gets updated automatically and easily!!
Things to be taken care of
1. Be careful with your selection. Take the references in such a way that there is least possibility of failing with its design intend.
2. Understand the how this works and select the boundary surfaces accordingly. For eg, if there is a chance that the pocket may get opened to the side when you modify it, then include the side surface also in the boundary surfaces, so that the feature will not fail when you make such modification.
