Working with Neutral Format Surface and Solid Models in Autodesk Inventor JD Mather Pennsylvania College of Technology Session ID ML205-1P In this class we will learn how to utilize neutral format data such as IGES, STEP and ACIS files in Autodesk Inventor. Particular attention will be focused on techniques for repair of flawed data in the Inventor Construction Environment. The Feature Recognition functionality for imported neutral and proprietary format files will also be covered. About the Speaker: Dr. JD Mather is an Assistant Professor of CAD & Product Design at Pennsylvania College of Technology, Penn State. He previously worked in industry for 15 years, including positions as journeyman machinist, research and development technician, and industrial engineering technician. Dr. Mather has been an Autodesk Inventor Certified Expert since release 7. He is also a Certified SolidWorks Professional. Dr. Mather placed second for Autodesk Inventor in the AU 2006 Avatech Altogether Smarter Challenge, and he placed first in the same category at AU 2007. jmather@pct.edu
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Session Objectives After attending this session, you will be able to: Use ACIS files beyond version 7 in your Inventor models. Use IGES and STEP files in your Inventor models. Use composite surfaces in your assembly drawings. Use imported IGES and STEP geometry for creating tooling. Use the Inventor Construction Environment to repair some types of imported geometry problems. Target Audience This is a power-track session intended for users with advanced experience with Autodesk Inventor. Manufacturing/mechanical engineers, designers and those involved in Inventor training should attend. Introduction Working with neutral format files can be challenging. There is often no easy button solution. You must be willing to experiment and try many different techniques when your initial efforts are unsuccessful. In a 90-minute class I am very limited in what we can cover. The problems chosen for this class were picked for brevity in solution while still covering most of the available tools. In some cases the problems might appear rather trivial but that is because I have spent countless hours in preparing the presentation of their solutions. I have limited the problems to those that can be solved within Inventor without 3 rd party software (except for a single brief case with ACIS format files that I ll describe shortly). There is ample information available on the Internet on the history of the various file types including ACIS, IGES and STEP. This will not be a history class. 3
We are going to look specifically at some techniques for working with less-than-ideal geometry in neutral format files. Of course you should not have to learn or be concerned with these techniques if the geometry were ideal. But we don t always work in an ideal world. Step number one in addressing any geometry conversion problem is to communicate with the source vendor/customer. If you can work together towards a solution it should be easier to get a good neutral file from native geometry in the originating software than to repair geometry in different software. Open the file ML205-1P-1.dwg in AutoCAD and execute the List command on some of the geometry. The list command returns information that the file contains BODY s and it shades like surfaces or solids. You might want to add a bolt circle hole-pattern to the flanges, but editing operations cannot be performed on the geometry. Many AutoCAD 3 rd party add-ons create geometry based on the ACIS kernel. The geometry might not be editable without the 3 rd party add-on. 4
Side Note Before we continue, a tip about ACIS (*.sat) files. Autodesk products will read up to ACIS v7 files. An ACIS file beyond that version will need to be converted to v7. Refer to Spatial Technology Corporation for further information on Hoops ACIS Viewer and other ACIS information. Search Google for the Hoops ACIS Viewer. In Hoops, from the pull-down menu Tools>Options change the Export Version Number to v7.0 and save the file. Notice that the highest version listed is v15.0. ACIS is now beyond that version, so you might get a file that you cannot convert to v7.0. In that case your best recourse is to contact Spatial or contact the source of the ACIS file. They can set the ACIS version Option when saving the file in the software they are using to create the geometry. 5
Open the ML205-1P-1.dwg file in Inventor. Be sure to click Options and set the File Open Options to Import. Click Finish in the DWG/DXF Import Wizard. Special Tip for AU attendees: TBA The geometry imports as a Composite surface. Right click on the Composite node in the browser and select Copy to Construction. Then right click on the Composite node and select Delete. 6
You will now see a folder called Construction at the top of the browser. Right click on the folder and select Edit Construction. This will take you into the Construction Environment (CE). Notice that the Panel Bar changes to reveal a new set of tools for this environment. Expand the Construction folder and the 0 group. Right click on the Surfaces and select Quality Check and then click Examine and Done. No problems were found with the geometry. 7
Right click on the surfaces again and this time select Stitch, then Apply and Done. Notice that the geometry is now listed as Solids (1) in the browser. Right click on the Solid and select Copy Object. 8
Click OK with the options set as shown. Then click Return to exit the CE and return to the Modeling Environment. That completes this problem, save the file. Special Tip for AU attendees: Explain this stuff, including confusing error prompt in earlier releases. Open with ML205-1P-2.stp with Composite Group Mapping. Click Options when opening the file. 9
Inventor generates a translation report that you can use to get more information about the file. If the translation report does not open automatically you can access it by expanding the 3 rd Party node in the browser and double click on Translation Report. Close the file. We will re-open it with different Options. 10
Again, open the file ML205-1P- 2.stp this time with the options shown. We want to set our Group Mapping to Construction Group. Notice that the geometry imports as 2 solids in the CE. Enter the CE by right clicking or double clicking on the Construction folder. 11
Key tip: Change the selection filter from Select Faces and Edges to Feature Priority. Right click directly on one of the solids in the graphics window and select Copy Object. Click OK with the default options. 12
Return from CE and Save As with the filename Bracket and delete the Construction folder. Save again. Special Tip for AU attendees: TBA Go back to the original file and Save As with the filename Sensor. Delete the Construction folder and save again. You can now assemble the two parts in an iam file using Mate- Flush constraints between the respective parts XY, XZ and YZ planes. Now it s your turn, see if you can duplicate the steps from Problem 2 with Problem 3, ML205-1P-3.igs. Note that you can assemble the parts in an iam using Mate-Flush with the respective part xy, xz, yz origin workplanes. Problem 2 was a STEP file while this one is an IGES file. 13
Open Problem 4, ML205-1P- 4.igs and right click on the Surface1 in the browser. Select Copy to Construction and then delete the surface feature from the modeling environment. Switch to the Construction Environment. Right click on the surface and Unstitch. As usual run a quality check. 14
Stitch the surfaces back together. We find a missing surface in the part. It appears that the part is symmetrical so maybe we can use a mirrored surface to repair the solid. First we try a simple Boundary Patch, but that doesn t work, so let s see how to mirror the missing surface. First we need to isolate the surface that we intend to mirror. We can do this by right clicking on the surface and select Move to Group. In this case we have an empty group. If necessary we could have selected Create New Group. 15
Stitch the remaining surfaces and RMB Copy Object. Set the Output to Create New Surface and Delete Original. Repeat this process for the isolated surface. Uncheck Translucent for the two copied surfaces. Create a new Workplane through the center of the part by clicking on the two planar faces on either side after starting the command. Use the workplane to Mirror the surface feature to the other side. Use the Stitch command to create the solid. 16
Tip: Perhaps you need the newly stitched solid in dwg format for a customer or vendor. Select the Applications>AEC Exchange pull down menu. Open ML205-1P-5.stp with the Options as shown. Our part translates as a solid but doesn t appear to be correct. Close the file. 17
Open ML205-1P-5.stp again, this time with the Options as shown. (Tip: These are the initial options I use when opening any IGES or STEP file that I m not sure of the content. The reason I do this is because opening a file with Auto Stitch and Promote turned on can take anywhere from minutes to hours. There is no point in using the Post translation options if a quick visual inspection indicates that the geometry is hopelessly flawed.) The geometry imports as surfaces in the CE. Run the Quality Check. 18
Delete the loop features as shown. (Recall how to set the Feature Priority selection filter?) Stitch the surfaces. Copy the 2 stitched surfaces to the ME using the following options. Select the Output as Create New Surfaces and Delete Original. 19
Create Boundary patches to close up the open rings on both ends. Stitch the surfaces into a disjointed solid. Alternatively you could use Sculpt. 20
Start a new sketch on the YZ Plane and Project Geometry the axis in each hole. Hit F7 for Slice Graphics and sketch the line and arc shown. Add tangent constraints between the lines and the arc as needed. Change the lines to Construction linetype. Start a sketch on one of the ring faces and Project Geometry the two circular edges. Sweep the sketch as shown. We had to create 2 sketches to fix this part. Now let s look and another method that does not require the creation of any sketches. Next we look at an alternative technique to fix this part. 21
Open the file ML205-1P-5.stp as done previously and delete the two outer torus features. Stitch the surfaces and promote (Copy Object) the surface to the modeling environment. Measure the distance from the inside cylindrical surface to the outside cylindrical surface. Thicken/Offset the arced surface. 22
Sculpt the surface. Open ML205-1P-6.igs with the options shown. If we expand the Construction folder notice that there are 2 Solids, 1 Surface and 2 Wires. Close the file. 23
Now open the file ML205-1P-6.igs with the indicated settings (see Group Mapping). Notice this time we have 3 Solids and the 1 Surface. The solids are easy to promote as we have done previously so we will isolate the surface and concentrate on that repair. 24
First I Unstitch the surface and then run a Quality Check. The Diagnostics indicates 4 problems. RMB to find the problem. I will click on each BODY and select Refit face. Repeat the Quality Check and Stitch to a solid and promote. 25
Open ML205-1P-7.igs with the Create Groups From: Levels (Layers) option. We already know how to separate out the two solids into different ipt files so I ll leave that to you. RMB on the Group and Group 3 and uncheck visibility. Group 3 contains wires that you might need for some reason. We will not use them. Also turn off the visibility of the 3D sketches. Enter the CE and RMB on the Construction folder and Define New Group. With the selection filter set to Feature Priority select the smaller part, RMB and Move to Group the newly created empty group. Turn off the visibility of Group 2, the green part, leaving only the smaller blue part visible. 26
Unstitch the surface and then run a Quality Check on the resulting 309 surfaces. If you Stitch the surfaces you will get a solid but it has some sliver faces that I don t think were part of the original design intent. (Actually, this appears to be a bit random at least one time I got a solid as shown, but usually I get a surface body.) You will have to use the Select Other tool to select and then delete these sliver faces. You might have great difficulty in locating them. There are a total of eight sliver faces located in two different areas of the model. You can locate them by rotating the model around and look for darker areas where there are multiple surfaces over top of each other. Stitch the part up again and the gaps will be closed. Promote the solid and save the file. 27
Make the other surface in the CE visible again and Unstitch, run the Quality Check and then try to Stitch back up to a solid. Two free edges will be found. RMB on one of them in the Stitch dialog box and select Find In Window. (Note: Undo the Stitch if it is back to 1 surface, you should have 136 surfaces.) Click the Extract Loop tool and checkmark Delete Wires in the dialog box. Select the surface shown and click Apply and Done. Move the resulting untrimmed surface into a new group and Stitch the remaining 135 surfaces together. Copy object the two surfaces (one is the 135 stitched, the other is the untrimmed) as surfaces to the ME. You could use the Trim Surface tool to trim back the surface to the correct boundaries, but this step isn t really necessary. The Sculpt tool will find the enclosed volume. 28
Open file ML205-1P-8.igs with the options shown. Our assembly browser fills up with parts but the graphics window is empty. If we double click on the parts in the browser we see that the parts are surfaces in the CE. 29
Open the file again with Auto Stitch and Promote turned on. Save the file. All of the parts except one are base solids. Start a new idw and create an isometric view of the assembly. Notice that part number U-6, the surface part, is missing from the view. Expand the part and RMB on the surface feature and select Include. The surface will now appear in the drawing. (Note: Earlier if we had tried to create a view of the assembly when all parts were surfaces we would have gotten an error we must have at least one solid in the assembly.) 30
However, we can create an idw of a single part that is only surfaces. We open the U-6 surface file and go through our usual steps of unstitching and running Quality Check in the CE. There are no errors returned but a visual inspection reveals suspect geometry. We can Extract Loop (un-trim) the questionable surfaces but the result is spheres that for this design would be difficult to re-trim. Isolate the questionable surfaces into a group by themselves. Special Tip for AU attendees: TBA Stitch the remaining surfaces and then copy to the ME as surface. 31
Start a new sketch on the xy-plane. Project Geometry the larger sphere edge as construction linetype and sketch the constrained arc as shown. Start a new sketch on the yz-plane and Project Geometry the smaller sphere as construction linetype and sketch the constrained arc as shown. Revolve the two arcs and then attempt to Sculpt the two revolved arc surfaces and the original stitched surface. The operation has no effect on the part. Extend the 4 edges as shown. 32
Try the Sculpt again and now we get a solid. The obvious question is, How did you know to extend those 4 surface edges? For those of you in attendance at AU I will show you the trick to identifying a case like this. Open file ML205-1P-9. You might have a zero thickness part for which you need to make tooling. I start by removing some of the holes in the CE with the Extract Loop command. 33
Some of the other holes are closed with the Boundary Patch command in the ME after creating sketch geometry. Once a sketch boundary is established we can Extrude To Next. Open file ML205-1P-10.igs. For this problem we need the 3D path centerline of the tube. The tube is a series of cylinders with torus segments connecting the cylinders. 34
Open the file ML205-1P-10.ipt that I have already started for you. Change the lines to construction and place a sketch point near the apparent intersection of each set of lines. Add coincident constraints to find the true intersection. Go to Tools>Document Settings and set the 3D Sketch Auto-Bend Radius to 100mm. (I ll explain later how I arrived at this radius.) 35
Start the line command and RMB make sure the Auto-Bend is turned on. Click on the line endpoint away from the arc and then the sketch point, continue on selecting the only the sketch points until reaching the other end of the tube. Once you have the 3D centerline you can use the Measure>Loop Length to find the length. Start a new metric file and Derive Component the solid body and the 3D sketch. With a bit of work a toolbody for creating a mold for the tube can be generated. It takes some time to set this up so I will simply show the steps on an existing file. 36
Once the toolbody is created it is used to create both sides of a mold with a complex split line. Sometimes it can be a bit more difficult as the 3D sketch will not find the center of the circles on the end of the cylinders. Recall that an arc is a planar entity. Also recall that a plane can be defined by two intersecting lines. We can use the axis of each cylinder to define the plane of the connecting torus segments. 2D sketches with Project Cut Edges can be used to establish the centerlines. 37