Posts tagged wizoscript
This tutorial demonstrates how to create a library of parts in a CAD neutral format based on a single template part. It takes advantage of parameterization in Geomagic Design.
We will start by creating the base part that we will use to create the library. This will be a simple cap head bolt.
Next we will use WizoScript to generate a library of 10 bolts of different lengths.
This type of task is ideally suited to scripting because it handles the tedious repetitive operations needed. While the part demonstrated in this tutorial is simple the same principles can easily be used for complex parts with multiple parameters.
Creating the Template Part
In Geomagic Design create a new part and then a sketch on the XY-Plane. On this sketch draw a circle centered on the origin with a diameter of 4mm and then extrude into a cylinder with a length of 10mm.
Under the Viewing and Analysis tab click on the Equation Editor button.
Double-click on “D2” and enter “Length” to give the length of the bolt a useful name then close the equation editor window.
Create the bolt head by adding a sketch to the end of the cylinder on the XY-Plane, setting the diameter to 8mm and extruding 4mm.
Create a new sketch on the top of the bolt head, draw a hexagon with an inside diameter of 4mm and then extrude cut 2mm.
Create a new folder called “PartLibrary” and save as TemplatePart.AD_PRT. Keep the part open in Geomagic to continue with the tutorial.
Writing a Basic Script
Start WizoScript 1.70 or later. When it runs it automatically creates an empty script that we can start using right away.
First we need to tell the script about our template part. For this tutorial the part must be open in Geomagic when the script runs, however it is possible to use a saved part that is not currently open. Please see the WizoScript reference manual for further details.
The following script line tells WizoScript “I have a part open and I want you to use it”:
TemplatePart = Part(“TemplatePart”, False)
Next we need to get access to the length parameter that we have already created it. Once we have access to it we can change its value
Length = TemplatePart.GetParameter("Length")
The default units for a script are millimeters, so if we enter the following:
Length.Value = 10
Then we are setting the length of the bolt to 10mm. Enter this into the script.
Now that we have set the length of the bolt we need to export it in a CAD-neutral formal so it can be shared with others. Here is how to do it:
This is what you should have so far:
Save the script and click on the Run button. If there are any errors correct them in the script and try again. If the script is successful you should now have a M4-Bolt-10.stp file.
Generating Multiple Parts
So far it’s not very interesting. We’ve generated a single STEP part that we could have easily created directly in Geomagic Design without needing scripting. Now we will look at generating multiple parts in one go.
The first step is to create a function that is given a length and creates a STEP file. A function is a way of grouping parts of a script together so they can be run over and over again. Edit your script to look like the following:
def GenerateBolt(NewLength): Length.Value = NewLength TemplatePart.ExportSTEP214("C:\Users\Andy\Desktop\M4-Bolt-"+str(NewLength)) TemplatePart = Part("TemplatePart", False) Length = TemplatePart.GetParameter("Length") GenerateBolt(10) GenerateBolt(12)
We now have a function called GenerateBolt that takes a length and creates a STEP file. The function has to be defined before it is used so put it at the start of the script.
Another key change is that the name of the STEP file contains the length, whatever that may be. This is achieved by appending “M4-Bolt-“ with the length value.
Run the script. It will call GenerateBolt twice and create two STEP files containing a 10mm bolt and a 12mm bolt.
The final step is to create a loop that goes from a minimum length to a maximum length creating bolts. Replace the two calls to GenerateBolt with the following:
MinimumLength = 10 MaximumLength = 20 for NewLength in range(MinimumLength, MaximumLength + 1): GenerateBolt(NewLength)
Run the script and it will generate bolts with lengths from 10mm to 20mm.
Here is the final script with comments added to explain:
# Takes a template bolt and creates a library of bolts of different lengths in # a CAD neutral format # Creates a bolt of a specific length. NewLength = desired length of bolt in mm # Saves the bolt to the desktop as a STEP file def GenerateBolt(NewLength): Length.Value = NewLength TemplatePart.ExportSTEP214("C:\Users\Andy\Desktop\M4-Bolt-" + str(NewLength)) # Get access to currently opened part that we will used as a template TemplatePart = Part("TemplatePart", False) # The template part has a Length parameter defined which we will control Length = TemplatePart.GetParameter("Length") # Create bolts from 10mm to 20mm MinimumLength = 10 MaximumLength = 20 for NewLength in range(MinimumLength, MaximumLength + 1): GenerateBolt(NewLength)
The Cooke Triplet is a system of three lenses designed in the 19th century to reduce distortion. In 1950 a specific triplet was invented and patented by Eastman Kodak (EF=100mm, f/1.9) and we will look at how to recreate it in Geomagic Design using scripting. We will create a script that can generate any type of thick lens, including how to solve the lensmaker’s equation. Hopefully the techniques demonstrated here will be useful to others solving and creating mathematical shapes in Geomagic Design.
Download, install and run WizoScript 1.70 or later. Start Geomagic Design. This script was tested with version 188.8.131.5290.
First we must enable a couple of useful libraries and make sure our script is using millimeters to match the values in the patent.
import sympy from sympy import * import math Units.Current = UnitTypes.Millimeters
We are going to generate three lens parts and save them so we need to specify a location to save to. Change this to make your PC.
OutputFolder = "P:\\temp"
The patent completely describes the three lenses but we are going to make it a bit more interesting by calculating the radius of the back of the lens from the focal length. To do that we need to use the lensmaker’s equation.
In the formula the radius of the back of the lens is R2. This appears in two locations in the formula. We could rearrange it to give us R2 = … but that is a bit tedious. Instead we can leave WizoScript to worry about it instead. Here is how we enter the equation into the script using ‘rb’ to represent the radius of the back of the lens.
# calculates the back radius of a lens based on the other parameters # uses the lensmaker's equation def GetBackRadius(FrontRadius, Thickness, RefractiveIndex, FocalLength): rb = Symbol('rb') Equation = Eq((RefractiveIndex-1)*((1/FrontRadius)-(1/rb)+(((RefractiveIndex-1)*Thickness)/(RefractiveIndex*FrontRadius*rb))),(1/FocalLength)) # we don't bother rearranging the equation, instead we let the sympy module do that for us BackRadius = solve(Equation) return BackRadius
WizoScript rearranges the equation and calculates the value we need using the single line:
BackRadius = solve(Equation)
The equation is placed into a function called ‘GetBackRadius’ which calculates the value when given a set of parameters, such as the thickness of the lens, refractive index of the material, etc. We can call the function repeatedly for different parameters.
Now we need to start creating a part for a single lens. First we tell Geomagic Design to create a part. We are going to do that in a new function.
# creates a part representing a lens based on a set of parameters def GenerateLens(Name, Folder, FrontRadius, Thickness, RefractiveIndex, FocalLength, Diameter): # get missing parameter BackRadius = GetBackRadius(FrontRadius, Thickness, RefractiveIndex, FocalLength) # check diameter is small enough if Diameter > abs(FrontRadius): print "%s diameter is larger than the front radius %f" % (Name, FrontRadius) return if Diameter > abs(BackRadius): print "%s diameter is larger than the back radius %f" % (Name, BackRadius) return # create new part Lens = Part(Name)
The general approach we will take is to draw a 2D profile of half of the lens on the XY plane and then create a revolve boss around the X axis. The X axis is the optical axis (i.e. the center of rotation for the lens).
# start creating the 2d sketch representing the shape of the lens Profile = Lens.AddSketch("Profile", Lens.GetPlane("XY-Plane")) LensRadius = Diameter / 2.0
First we will draw the front of the lens. There are three possibilities, the front is flat (infinite radius), bulging out aka convex (positive radius) or indented aka concave (negative radius). We treat each case individually. Simple trigonometry is used to calculate the end points of the front. Note that infinity is represented in the script by ‘oo’.
# draw shape of the front of the lens, it can be flat, convex or concave if FrontRadius == oo: FEndX = 0 Profile.AddLine(0, 0, FEndX, LensRadius, False) elif FrontRadius > 0: Angle = asin(LensRadius / FrontRadius) FEndX = FrontRadius - (cos(Angle) * FrontRadius) Profile.AddArcCenterStartEnd(FrontRadius, 0, FEndX, LensRadius, 0, 0, False) else: FrontRadius = -FrontRadius Angle = asin(LensRadius / FrontRadius) FEndX = (cos(Angle) * FrontRadius) - FrontRadius Profile.AddArcCenterStartEnd(-FrontRadius, 0, 0, 0, FEndX, LensRadius, False)
The back of the lens is treated in the same way except the sign of the radius is reversed. This means that a convex shape is a negative radius and a concave shape is a positive radius.
# draw shape of the back of the lens, it can be flat, convex or concave if BackRadius == oo: BEndX = Thickness Profile.AddLine(Thickness, 0, BEndX, LensRadius, False) elif BackRadius < 0: BackRadius = -BackRadius Angle = asin(LensRadius / BackRadius) BEndX = (cos(Angle) * BackRadius) - BackRadius + Thickness Profile.AddArcCenterStartEnd(Thickness - BackRadius, 0, Thickness, 0, BEndX, LensRadius, False) else: Angle = asin(LensRadius / BackRadius) BEndX = -(cos(Angle) * BackRadius) + BackRadius + Thickness Profile.AddArcCenterStartEnd(Thickness + BackRadius, 0, BEndX, LensRadius, Thickness, 0, False)
Before we can add the revolve boss we must make sure the sketch is closed by drawing the line for the outside of the lens and the line along the optical axis
# check diameter of lens again if FEndX > BEndX: print "%s diameter is too large" % Name return # if this is not a "thin" lens then draw top of profile if FEndX != BEndX: Profile.AddLine(FEndX, LensRadius, BEndX, LensRadius, False) # draw line of profile along x axis (optical axis) Profile.AddLine(0, 0, Thickness, 0, False)
Now for the revolve boss.
# create lens by revolving sketch around x axis Lens.AddRevolveBoss("Lens", Profile, Lens.GetAxis("X-Axis"), 360.0)
Creating two reference planes for the front and back of the lens will help with aligning them to create the triplet. Finally we save and close the part.
# add reference planes to aid in aligning this lens with others Lens.AddPlane("Front", Lens.GetPlane("YZ-Plane"), 0); Lens.AddPlane("Back", Lens.GetPlane("YZ-Plane"), Thickness); # save and close Lens.Save(Folder) Lens.Close()
The last step is to generate the three lenses needed for the triplet using the values from the patent along with the focal length.
# lens 1 GenerateLens("Lens1", OutputFolder, 62.63, 25.56, 1.745, 73.2, 40.0) # lens 2 GenerateLens("Lens2", OutputFolder, -66.47, 4.51, 1.647, -37.74, 36.0) # lens 3 GenerateLens("Lens3", OutputFolder, 119.5, 19.92, 1.697, 54.88, 30.0)
The complete script can be obtained from the script library. Running it will generate three part files, one for each lens.
Create a new assembly and add the three lenses in the order lens1, lens2 and lens3. Align the X axis of all three lenses. Align the front plane of lens2 7.89mm from the back plane of lens1. Align the front plane of lens3 14.14mm from the back plane of lens2.
This mini tutorial shows how to generate custom Mobius strips with minimum effort. It demonstrates that python scripting can be used to ask the user for information and then apply it to a part the user is already working on. Hopefully that will be useful to some people when solving problems.
1. Download and install WizoScript 1.70 or later and start it.
2. Start Geomagic Design V16 hotfix 1 (184.108.40.20690) or later.
3. Create a new part and set the units to millimeters.
4. Create a new sketch on the XY plane.
5. Draw a triangle centered on the X axis and set the size of the reference circle to 10mm.
6. Set the center of the triangle 30mm from the origin and exit sketch editing mode.
7. Go to the WizoScript script library and copy the Interactive Mobius Strip Generator. Paste it into WizoScript. Hint: double-clicking on the script in the web-page selects the entire script.
8. Run the script.
9. You will be asked for the name of the part. Assuming you haven’t saved it enter “New Part (1)”. Then you will be asked for the name of the sketch. Enter “Sketch<1>”.
10. Next you will be asked the rotation point along the X axis. Enter “30”. This puts the rotation point at the center of the triangle.
11. You will be asked for the number of rotations. This is the number of times the mobius strip will completely rotate. Enter “3”.
12. Finally you will be asked to enter the number of steps. Enter “30”.
Now the mobius strip will be generated. Be patient as this can take several minutes. Here is what you should have:
Now it’s time to experiment! You can change the shape of the sketch to create different effects. Setting the rotation point closer or further away from the origin will create a “corkscrew” effect. You can increase or decrease the number of rotations. Reducing the number of steps will make the part faster to create but you might have to manually add a guide curve to get a true mobius strip.
Using this script it is possible to run it multiple times on the same part. For example create two sketches, run it on the first sketch and then run it on the second sketch to create two Mobius strips that are intertwined.