Pro/E Manufacturing Tutorial

This is a tutorial for the manufacturing side of Pro/E Wildfire 4.0, which the lab has been slowly migrating to. The contents of this tutorial are meant to replace our use of Unigraphics. Part Modeling is discussed ad nauseum many other places, so we're mostly focusing on BDML-specific manufacturing issues with this tutorial.

View the Manufacturing Tutorial video to see the talk
See ProESetup for installation instructions
Go to the Haas Info page for more information about HAAS-specific things.

BDML-specific and HAAS-specific setup procedures

Save and extract the necessary BDML Pro/Engineer Setup Files from the Twiki
In Windows explorer, navigate to the C:\ drive. Check to see if there is a directory called "C:\BDML". Clear out everything in this directory(Pro/Engineer has to be closed to be able to)
Inside the .zip file, move everything in the BDML directory into C:\BDML. Everything Pro/Engineer needs is contained within this directory.
Finally, you need to modify the Pro/Engineer Shortcut in the start menu to point to "C:\BDML".
1. Open up the start menu, navigate to the Pro/Engineer icon
2. Right click on the icon and open up the properties.
3. In the "Start In" field, type C:\BDML (image)

the default speeds/feeds contained in "haas.gph" are for wax machining, and must be edited if we switch materials!! If the tools within the HAAS change, if we want to make a template for machining with different fixtures, or if we start using materials other than wax, these settings must be changed!

Before we start

You absolutely need a three-button mouse
1. used for rotating your view
2. need the center button for dimensioning sketches
ctrl-d is the default trimetric view
the view buttons along the top allow you to toggle various workspace items on and off, as well as select how to orient and shade your workspace.

Creating a wax block cutout part

open pro/e from programs/ptc/pro-engineer (image)
start a new assembly (image)
1. select Sub-type > Design and make sure that the "Use default template" box is unchecked (image)
2. name the assembly and click OK
3. select from the template list "mmns_asm_design" and click OK
Insert necessary parts
1. Go to insert > component > assemble (image)
  1. insert a blank wax block part, we'll call this part: waxblockblank.prt
  2. make sure the blank wax block part is 12" by 12" on the top face and taller than the solid part you want to make the cutout from
  3. select "Default" for the constraint and click the green checkbox (image)
2. Go to insert > component > assemble (image)
  1. insert the solid part you want to use to make the wax block cutout, we'll call this part: solidpart.prt
  2. fully constrain solidpart.prt to waxblockblank.prt
    1. make sure that the top faces of solidpart.prt and waxblockblank.prt are aligned (image)
    2. finish constraining solidpart.prt in the place where you want to remove material from the wax block. it should be completely inside of the wax block (image)

Make wax block cutout part from existing two parts
1. Go to insert > component > create
  1. type: part, sub-type: solid, we'll name this newpart.prt (image)
  2. creation method: empty, uncheck "Leave component unplaced" and click OK (image)
2. Right click on newpart.prt on the parts tree in the left column. From the right-click menu select "Activate"
3. Insert > shared data > merge/inheritance (image)
  1. Click waxblockblank.prt
  2. Click the green check box to accept
4. Insert > shared data > merge/inheritance (image)
  1. Click solidpart.prt AND click/highlight the "Remove Material" button (image)
  2. Click the green check box to accept

Your wax block cutoutpart is now complete (image)
SAVE YOUR FILE!!!

Beginning a manufacturing assembly

start a new manufacturing assembly (image)
1. select nc assembly (image)
2. make sure you name it a unique name. it will be hard to rename later. (image)
3. make sure you deselect "default template" (image)
4. hit enter
select from the template list mmns_mfg_nc. This will establish the units of the manufacturing assembly as metric. (image)
1. despite the fact that inches should work just as well in the HAAS, it has not been thoroughly tested. Therefore make sure your manufacturing project is in mm.
2. if you forget this step you can redefine it later. Here's how:
  1. Go into the manufacturing window on the right, (image)
  2. select setup->units and set mmns as the new units, then hit set (image)
  3. you will be given the option to pick whether you convert all your dimensions from inches to millimeters by multiplying byt the conversion factor, or by reinterpreting the dimensions in the new unit. (image)

Your new assembly will open up (image)
1. the hierarchical window on your left is your assembly navigator. In this window you can hide parts, suppress steps, etc, very similar to solidworks. (image)
2. the window on your right is the manufacturing window. This window takes you through the steps of setting up your manufacturing sequence. (image)
3. The center area is the workspace where you can create and import parts and assemblies to define your manufacturing sequence (image)
4. The icons to the right of the workspace are tools you can use in the current application.
SAVE YOUR FILE!!!

Setup the project

first we want to create/define all of the parts we are basing our milling operations from
* ref model is the final part we want to create. we have to define at least one ref model
* workpiece is the original "blank" that the final block is made from. It is useful to define this part if the blank has interesting geometry. it isn't necessary to define a workpiece.
1. in the manufacturing window, click on manufacturing model (image)
2. click assemble (image)
3. click reference model (image)
4. find the part you want milled (image)
5. The part will be imported into the workspace, and a dialog window will drop down from the top and help you place the part. (image)
  1. select fix to fix the part where it is (image)
  2. select default to fix the part so that part and assembly coordinate systems match up (image)
  3. select automatic to dynamically create constraints to other parts or assemblies (image)
    1. in automatic, you can create constraints by clicking on points between two parts and establishing new constraints.
    2. the placement and position tabs can help you further define your mating conditions.
    3. constraints can be removed once they have been added using the placement window.
      1. Right click on a specific constraint to remove it.
    4. When finished, the status bar in the top dialog should say %u201Cfully constrained%u201D
  4. click on the green check mark to accept. (image)
  5. to get back to these settings later, go to the part you imported in the assembly navigator and right click "edit definition"
6. a new dialog will pop up. this dialog determines how the original part file is linked to the manufacturing assembly. (image)
7. click ok to accept default settings.
8. Click done in the manufacturing window (image)
9. SAVE YOUR FILE!!!
  * You can bring in multiple reference parts. repeat above steps to do so
  * Workpieces are also brought in using the same steps
next, we want to define a new CSYS for the center-top of our 12"x12" wax block.
* the z-axis must always point up out of the top of the block. This is the axis along which all the mills are oriented, and the axis along which they spin.
* the x and y axes must always be positioned 6" from the edges of the block. The x-y plane must be on the top(cutting) surface.
1. Click on the CSYS button. (image)
2. A dialog will pop up which will allow you to position your new CSYS based on existing planes, features and Coordinate systems (image)
3. select the default CSYS in the assembly navigator, and enter the offset of the new one.
4. name the new CSYS MachineHomeG55 (so I can refer to it later in this tutorial) (image)
5. hit ok
6. SAVE YOUR FILE!!!
  * alternatively, when defining the mating conditions of your imported ref model, you could have positioned your ref model so that the CSYS was positioned in the top-center of the wax block, eliminating the need to create a new one. This is just easier to do after the fact.
Now we want to go to the manufacturing setup item to define our cnc machine, our tools, fixturing, etc. To do this we define a new operation.
* An operation is defined as everything you can do while fixtured in a single mill or lathe.
* If you unclamp your part, reorient it, and/or put it into a new machine, you need to define a new operation.
* you can use multiple tools and create separate toolpaths within the same operation.
1. Click on manufacturing setup->operation (image)
2. the operation is automatically named OP10. You can rename it if it makes sense. (image)
3. click on the machine tool setup icon. A new window will pop up. (image)
4. Open haas.gph. This loads the HAAS parameters (image) (image)
5. Tools for the HAAS are defined in haas.gph, however you can also save and load individual tools as well if we do frequent tool swapping. This is done via the cutting tool tab of the machine setup page. br>* To get to the tool page, click on head 1. (image)
  * The tool page is important to set up correctly, because by using appropriate parameters we can ensure safe cutting
  * it's important to fill in all the information you have on the tool when adding a new one. (image) (image) (image)
  * tool #/offset# need to be the same, and are used by the postprocessor for Tx / Hx.
  * cut data - you can specify speeds/feeds for roughing and finishing, which can later be imported straight into your nc operation setup.
6. Accept the machine dialog window
7. Back in the operation dialog, click on the arrow next to machine zero, then select the new CSYS we created earlier, MachineHomeG55? . You can select it either in the workspace or in the assembly navigator (image)
8. click on the arrow next to retract plane, and enter 10 to define the clearance plane 10mm above the wax block. (image) (image) (image)
9. make sure the "always use operation retract" option is checked. (image)
10. Accept the operation dialog
11. Click done in the manufacturing window (image)
12. SAVE YOUR FILE!!!

Select the material to remove

there are many ways to define which material we will be removing. Two of those types of definitions are mill volumes and mill windows.
* mill volume is a special 3d solid body you create with your standard solid modeling tools.
* mill window is a special 2d shape which provides a planar entry point for material removal.
1. To create a mill volume
  1. select the create mill volume icon from the toolbox to the right of the workspace (image)
  2. a dialog box will drop down from the top
  3. it's a good idea to hide the parts you don't want to work with at this point.
  4. create a new sketch by selecting the sketch icon (image)
    1. a constraints/placement dialog will pop up (image)
      1. a. select the top plane of the wax block to define the sketch plane (image)
      2. hit sketch to close the window
    2. a references dialog will pop up.(image)
      1. select a reference point or edge, such as your Machine CSYS (MachineHomeG55) to reference dimensions from. (image)
      2. hit solve. the sketch should now be completely constrained. (image)
      3. Continue to select lines and vertices from the part which you will use for positioning your new sketch. You can do this at any time.
      4. You can come back to this menu in sketch mode by selecting sketch->references from the top menu.
    3. draw a box around the volume you wish to mill with the rectangle tool (image) (image)
      * notice that dimensions and constraints have been automatically added, fully constraining your sketch immediately.
      1. Automatic dimensions are in gray.
      2. Double click on any automatic dimension to edit the value. Any specified dimension is no longer automatic, and shows up in white.
      3. other dimensions can be created using the dimension tool.
    4. you should now constrain the edges of your rectangle to the edges of the volume you wish to mill(image)
      * if you don't do this, changes to the base part will not change the dimensions of the mill volume if they grow outside the bounds of the rectangle you drew.
      1. select the constraints tool (image)
      2. select the colinear, vertex, alignment tool (image)
      3. select the top edge of the rectangle (image)
      4. select the topmost edge or vertex of the volume you wish to remove. You can select the top edge or vertex of the wax block to constrain your rectangle to that if you wi
      5. the sketched rectangle should have changed its top edge to align with the top edge of the part.
      6. repeat this step for each edge of the rectangle
    5. click the check mark in the sketch to leave sketch mode.
  5. select insert->extrude. (image)
    1. a dialog box will drop down.(image)
    2. edit your extrude options to extrude through the entire depth of the volume you want to mill
    3. click the green check mark (image)
  6. select the trim tool on the right (image)
    1. select the ref model (solid body) you would like to trim your extrusion from.
  7. click the green check mark to accept your mill volume. (image)
2. To create a mill window,
  1. select the create mill window icon from the toolbox on the right image)
  2. a dialog box will drop down from the top (image)
  3. it's a good idea to hide the parts you don't want to work with at this point.
  4. click on the top face of the part you want to place your window on
    * if you have defined multiple ref models, you need to specify which part you're clicking on.
    * this is indicated by the red placement tab.
    (image)
    1. click the ref model you're placing your window on.
    2. go to the depth tab, and select "specify depth"
    3. select the bottom surface you would like to extrude to, or enter an offset.
    4. click on the green check mark (image)

Generating Toolpaths

Before we begin, hide the mold part such that only your final parts are shown (hide the .prt entry and leave the trim visible)
next we want to create an sequence of nc commands for removing material.
1. click on machining (image)
2. click on nc sequence (image)
3. select volume milling (image)
4. a set of checkboxes will pop up. (image)
  1. The elements that are checked are the elements you want to view/modify in your NC sequence.
  2. Make sure tool, parameters, and either volume or window are checked, and hit done.
5. the tool selection dialog will pop up. (image)
  1. Select the tool you want to use.
  2. Hit ok
6. the parameters dialog will pop up
  * you can enter all the machining values manually, or
  * you can bring in the default parameters for the tool you selected
  1. to do this hit edit->copy from tool->all->rough(or finish) (image)
  2. define the remaining required parameters (image)
    * clear dist - this is the distance above the part the mill slows down to cutting speed. specify at least 3mm.
    * RETRACT_FEED - not necessary, but really speeds up the process. Set it to 2000
    * Tolerance - The Haas's tolerance is .001 mm. You should use this value unless you don't care about the precision of your cut and want to shorten computation time

1. 1. redefine any other parameters, including
    * scan type
    * rough option
    * you can also switch between "basic" and "all" parameters to edit more parameters
2. select the volume mill by selecting your parts in the window (not in the assembly navigator). (image) (Note: we need to double-check how to do mill windows!!)
3. your nc sequence is now fully specified. click done in the manufacturing window. (image)
4. SAVE YOUR FILE BEFORE PLAYING YOUR SEQUENCE!!! Sometimes Pro/E can take several minutes, even HOURS to compute; you want to have saved these last steps first.
5. in the assembly navigator on the left, right click on volume mill, and select play sequence.(image)
  * the sequence will be calculated, and a play dialog will pop up
  * you can play the entire sequence at any speed, as well as navigate to any point along the sequence to see more detail(image)
6. SAVE YOUR FILE!!!
if you wish to clean up your first path with a smaller tool, local mill is the nc sequence for you
1. select "nc sequence","new sequence","local mill", and "done"
2. select "previous nc sequence", "done"
3. select "one item", "NC Sequence", select the previous volume milling you just created
4. select "Cut MTN #1"
5. a set of checkboxes will pop up.
  1. Make sure tool and parameters are checked and hit done.
6. the tool selection dialog will pop up.
  1. Select the tool you want to use.
  2. Hit ok
7. the parameters dialog will pop up
  * you can enter all the machining values manually, or
  * you can bring in the default parameters for the tool you selected
  1. to do this hit edit->copy from tool->all->rough(or finish)
  2. define the remaining required parameters
    * clear dist - this is the distance above the part the mill slows down to cutting speed. specify at least 3mm.
  3. redefine any other parameters, including
    * scan type
    * rough option
    * you can also switch between "basic" and "all" parameters to edit more parameters
8. your nc sequence is now fully specified. click done in the manufacturing window.
9. in the assembly navigator on the left, right click on local mill, and select play sequence.
  * the sequence will be calculated, and a play dialog will pop up
  * you can play the entire sequence at any speed, as well as navigate to any point along the sequence to see more detail
10. SAVE YOUR FILE!!!
it is possible to to edit your nc sequences once you've created them.
1. go into the manufacturing menu
2. click machining->NC Sequence
3. select the existing NC sequence you'd like to modify.
4. a set of checkboxes will open up. Select which features of your sequence you'd like to edit.
5. you can then make changes
6. SAVE YOUR FILE!!!

Fixing problems

If something changes in any of your base parts, conflicts in the related files may arise. You will be notified and be allowed to fix the offending geometry/constraints
1. the fix dialog will open on the right
2. select quick fix, and try to identify the element causing the conflict, and then use the tools in the fix dialog to update any faulty constraints.

Outputting GCode

finally, we want to output our NC Sequences to a set of G-code files
1. to output the entire operation
  1. in the main manufacturing window
  2. select "cl data"->"output"->"select one"->"Operation" (image)
  3. select the operation (image)
2. to output a single sequence
  1. in the main manufacturing window
  2. select "cl data"->"output"->"select one"->"nc sequence"
  3. select the specific sequence
3. to combine individual nc sequences into one file
  1. in the main manufacturing window click "cl data"->"output"->"create set"
  2. enter the name of the set and hit enter
  3. select the nc sequences you want to combine and hit done
  4. select the set you just created
4. select "output"->"file"
5. make sure "cl file", "mcd file", "interactive", and "compute cl" are checked (image)
  * "cl file" - outputs the intermediate .ncl file
  * "mcd file" - runs the postprocessor upon the .ncl file
  * "interactive" - opens the dialog window and allows you to enter the program number and see the results of the generation
  * "compute cl" - recalculates all the toolpaths in case anything changed.
6. click done. The paths will be recalculated
7. when done recalculating the .ncl, a new menu with postprocessor options will pop up
8. make sure verbose, trace, and machin are checked.
9. click done
10. a console window will open. Press enter to accept the default HAAS program number, or enter a new one.
11. click done
12. Your output files will be in the *.tap format of the name you specified while postprocessing.
13. SAVE YOUR FILE!!!

How to efficiently plane your wax block

1.This Section of the tutorial will cover how to modify the existing Wide Plane mfg to allow you to only have to use one, maybe two, tool paths to surface your wax block regardless of the amount of material that needs to be removed. This technique works by modifying the Wide Plane mfg to use repeated iterations of the toolpath to shave down layers. For this example we will generate a toolpath that will remove 50mm of material.

To start open ProE? and download this zipped file
After opening ProE? go to file open the downloaded WIDEPLANE01.mfg
1. This file already has the toolpath generated all you have to do is simply modify the parameters of the path to fit your specific needs.
2. After WIDEPLANE01.mfg has opened, open Mfg Setup in the manufacturing menu in the top right corner. (Image 1)
3. After selecting Mfg Setup in the manufacturing menu open the operations tab. (Image 2)
4. Next in the operation Setup window that has opened modify the surface retract distance by clicking on the arrow button. (Image 3)
5. This window is where you will rdit the distance that the tool will retract from the surface, this value scales with the amount of material you wish to remove. This scale is value mm = amount of material you want to remove (z direction)mm +10mm (standard retract distance). As you can see the value in this tutorial is set to 60, this is the amount of material we decided to remove (50mm) + the standard retract distance (10 mm). (Image 4)
After entering the correct value select OK -> OK -> Done until you have returned to the original mfg menu.
Now we must choose the number of iterations that you would like run.
1. To get to the screen to edit this select Machining-> NC Sequence. From there select 1: Face Milling, Operation: OP010. (image 5)
2. From this screen select SEQ SETUP check the box next to parameters and then select done. (image 6)
3. Next select the All button next to Parameters. (image 7)
4. Scroll down until you can select Number_Cuts (this is where you select the total number of iterations that you want). Remember that the max we should be taking off with the face mill is 2mm. So then you take your desired material to remove / the amount of material per pass = number of cuts.Ex. We want to take off 50mm for this example therefore we have 25 cuts. (image 8)
5. Select done and return to main manufacturing screen.
6. Output your G - Code as outlined in the section above.

References

	jhu_proE_install.pdf	This is a useful installation reference
	CAM_nd_logo_wf3.pdf	Step-by-step manufacturing instructions from Notre Dame
	UniversityofBridgeport-ME421-CAM.zip	Lecture Notes from a Manufacturing class that uses Pro/E
	ProE_Wildfire_2_Tutorial-2006.pdf	Useful tutorial from the University of Victoria
	getting_started_pro_e_wildfire.zip	A tutorial from PTC with samples and examples
	WF3_Manufacturing-0.swf WF3_Manufacturing-1.swf WF3_Manufacturing-2.swf WF3_Manufacturing-3.swf WF3_Manufacturing-4.swf	Tutorial Videos from PTC's tutorial website
	978-1-58503-415-4-2.pdf	Another tutorial
	wildfire-tips.pdf	wildfire-tips.pdf
	WF4QRC-Web.pdf	Wildfire 4 Quick Reference Card

Notes for Dan on the tutorial

We should emphasis rough option more clearly in step 18.k.iii. Or at least say that the default option, rough&prof, takes forever (like 5 pass over the same area over and over again) to cut simple stuff. scan type is also important, but this is more for the surface finish than the time using the haas.
To figure out the machining time:
- Right click on the operation (volume milling) --> info --> features
- Find Machining time under Manufacturing Info
Tutorial2.jpg:

Copyright &© by the contributing authors. All material on this collaboration platform is the property of the contributing authors.
Ideas, requests, problems regarding TWiki? Send feedback