Chapter 6: Importing Solid Models

Chapter 1 * Chapter 2 * Chapter 3 * Chapter 4 * Chapter 5 * Chapter 6 * Chapter 7 * Chapter 8 * Chapter 9 * Chapter 10 * Chapter 11 * Chapter 12 * Chapter 13 * Chapter 14

6.1 Importing Solid Models from IGES Files

As an alternative to creating a model directly within ANSYS, you can first create a solid model in your favorite CAD system, save that model as an IGES file, and then import that model into ANSYS. Once successfully imported, you can mesh the model just as you would for any model created in ANSYS.

6.2 Working With IGES Files

ANSYS provides the following two options for importing IGES files:

• DEFAULT-This option uses an enhanced geometry database and should, in almost all cases, be your choice. The option was designed to convert IGES files, if possible, without user intervention. The conversion includes automatic merging and the creation of volumes to prepare the models for meshing. If the DEFAULT option encounters problems translating the IGES file, ANSYS will alert you to this and activate a suite of enhanced topological and geometric tools designed specifically for interactive repair of imported models.
• ALTERNATE-This option uses the standard ANSYS geometry database, and is provided largely for backward compatibility with the previous RV52 import option. Occasionally, ANSYS will be unable to translate an IGES model using the DEFAULT option and you'll be instructed to try to ALTERNATE option. The ALTERNATE option has no capabilities for automatically creating volumes and models imported through this translator will require manual repair. However, the enhanced set of topological or geometric repair tools is not available for models imported through this translator; you must use the standard PREP7 geometry tools to repair your model. Instructions for this option may be found near the end of this chapter.

6.2.1 Using the DEFAULT Option

1. Import the model with automatic merging and volume creation turned on (the default conditions). For large files (of the order of 5 MB or more), increase ANSYS's memory allocation before importing the model.

2. General indications that a model requires manual clean-up include failure during merging or ANSYS requesting unreasonable amounts of memory. In general, if the file contains unnecessary (or infinite) entities, automatic merging will fail or ask for more memory. You can continue to the topological repair stage to delete the entities and continue with merging. Otherwise, you must

• Import the file without merging and volume creation.
• Go through the topological and geometry repair procedures to delete unwanted entities.
• Merge the model.
• Create lines and areas to replace missing entities.
• Create volumes.

Should the DEFAULT IGES translator encounter problems, ANSYS will advise you that you must use the topological and geometric repair tools to interactively complete the model. The following briefly covers the various tasks you may need to perform to prepare a model for meshing:

• Use the topological repair tools to close gaps between entities in the model. This should always be your first step in repairing models. ANSYS will not allow you to access the geometry repair tools until you explicitly declare that you are finished with topological repair.
• Repair incomplete entities to create lines, areas and then volumes. This generally means completing boundaries that can be "filled" with lines and areas (think of this as creating a line from existing keypoints or an area from existing lines). You can then force the creation of a volume from the completed areas.
• Enhance the geometry through the creation of geometric primitives and the use of Boolean operations. This may be necessary to rebuild geometric entities that could not be translated from the IGES file.
• Attempt to mesh the model as outlined in Chapter 7. If you discover meshing problems due to physical features in the model (very small lines, areas, or loops; areas that are disproportionately long in one direction; or other parameterization problems), you can simplify the model using the geometry simplification tools.
• Simplify geometry to improve meshing. For this task, you'll locate and remove "problem" features from the model.
• Attempt to mesh the model again. If you encounter further problems in meshing, you may need to further simplify the geometry.

The following sections cover each of the above tasks in detail.

6.2.2 Importing IGES files for the DEFAULT Option

Command(s):

IOPTN

Utility Menu>File>Import>IGES

• Select the Default option.
• Set Merge coincident keypoints to Yes (default)
• Set Create solid if applicable to Yes (default)

Command(s):

IGESIN

File picker dialog box that follows after setting IGES options.

Note-If you have already loaded an IGES file using the Default option, you must clear the database before loading a new IGES file.

There are several circumstances when you may wish to set the import options differently than above. You should not merge coincident keypoints or create solids if:

• There are geometric entities in the model that you know you will want to delete after transfer.
• The model contains surfaces which you know are not properly "trimmed." You should eliminate these surfaces in ANSYS before merging.
• The IGES model is very large. In such cases, it is often a good practice to import the model into ANSYS without these options active before attempting to merge keypoints and create solids.
• The model contains surfaces which don't share common boundaries. In such cases you may wish to separately mesh individual surfaces.
• The model you are importing is not a solid model.

Note-The SMALL option for the IOPTN command allows the user to specify whether or not small areas are deleted or included. In most cases, deletion of small areas can speed up the processing time and import models successfully. However, if your model is a thin shell model or contains important small areas, setting the value to "NO" can retain all of the small areas. This setting may cause increased processor time and memory usage.

Note-If your model is missing geometric entities, you may be able to restore them by importing the model again and setting the GTOLER option for the IOPTN command. The GTOLER option sets a multiplier value used to adjust the maximum dimension of the actual model (the maximum dimension affects internal tolerances in the translator). In general, if your model contains planes that are disproportionately large in comparison to the model itself, you should set the multiplier value such that the result is a dimension that is approximately the size of the model.

Note-For most cases, using the GTOLER option is not recommended. However, if your model fails to import successfully sometimes using the GTOLER option can help. In particular, setting a large multiplier value can help to eliminate small features in the model. Conversely, if your model is missing many small (but important) features, using a small multiplier value can restore these.

6.2.3 Repairing Topology

The topological repair tools provide the following capabilities:

• Setting preferences for the gap listing and plotting commands.
• Plotting open edges (gaps) only, closed edges only, or both open and closed edges.
• Listing open edges only or closed edges only.
• Merging gaps that fall within a specified tolerance.
• Merging as many gaps as possible through an automatic iterative merging process.
• Deleting geometric entities.
• Exiting from the topological repair tools.

You are forced to enter topology repair before accessing other geometry tools because in many instances problems within an imported model can be repaired by these tools alone. Even if the topological repair is not sufficient to create volumes in the model, these repairs should be done before working with the model's geometry.

Normally, you will use the following general procedure to repair the topology of your model.

1. Set preferences for plotting and listing tools.

2. Examine the model for gaps (through both listing and plotting).

3. Delete any unattached and unnecessary geometric entities (such as "bad" geometry and untrimmed surfaces).

4. Use the iterative merging tool to merge gaps.

5. Exit the topological repair tools and, if necessary, continue repairing the model through the modeling (geometry) tools.

6.2.3.1 Setting Preferences for Gap Plotting and Listing

Command(s):

GAPOPT

Main Menu>Preprocessor>-Modeling-Topo Repair>Preferences

There are two preference settings:

• TOLER-This sets the merging tolerance factor for the GAPPLOT, GAPLIST, and GAPMERGE commands. Each time you set the tolerance, ANSYS queries the database and generates an internal list of lines that can be merged within the specified tolerance. When you click either OK or Apply in the Topological Repair Preferences dialog, ANSYS will report (through a message box) if none of the gaps can be merged at that tolerance.
• OESELE-This sets the types of open edges (gaps) that are shown by the listing and plotting commands. You can specify that the commands will
  • List/plot all open edges, including both open edges that can and can't be merged.
  • List/plot only those open edges that will be merged.
  • List/plot only those open edges that will remain.

6.2.3.2 Finding Gaps

Using the Listing Functions

Command(s):

GAPLIST

Main Menu>Preprocessor>-Modeling-Topo Repair>-Lst Model Gaps-Open edges

To list all closed edges.

Command(s):

GAPLIST

Main Menu>Preprocessor>-Modeling-Topo Repair>-Lst Model Gaps-Closed edges

Using the Plotting Functions

• Blue - closed edges.
• Red - open edges that will remain open if the GAPMERGE command were issued with the current GAPOPT tolerance setting (note that the GAPOPT tolerance must be set separately).
• Yellow - open edges that will be closed if the GAPMERGE command were issued with the current GAPOPT tolerance setting (note that the GAPOPT tolerance must be set separately).

To plot all open edges that can be merged at the current tolerance setting:

Command(s):

GAPPLOT

Main Menu>Preprocessor>-Modeling-Topo Repair>-Plt Model Gaps-Open Edges

To plot all closed edges:

Command(s):

GAPPLOT

Main Menu>Preprocessor>-Modeling->Topo Repair>-Plt Model Gaps->Closed Edges

To plot both all open edges, disregarding the tolerance setting, and all closed edges:

Command(s):

GAPPLOT

Main Menu>Preprocessor>-Modeling->Topo Repair>-Plt Model Gaps->Opn & Closed

Figure 6-1 Open and closed plot showing gaps, shown as darker (red on the display) lines. These gaps are very narrow and appear as lines at this zoom level.

6.2.3.3 Deleting Geometric Entities

To delete keypoints not attached to a line:

Command(s):

KDELE

Main Menu>Preprocessor>-Modeling-Topo Repair>Delete>Keypoints

To delete lines not attached to an area:

Command(s):

LDELE

Main Menu>Preprocessor>-Modeling-Topo Repair>Delete>Lines Only

To delete lines not attached to an area as well as all keypoints attached only to that line:

Command(s):

LDELE

Main Menu>Preprocessor>-Modeling-Topo Repair>Delete>Lines and Below

To delete areas:

Command(s):

ADELE

Main Menu>Preprocessor>-Modeling-Topo Repair>Delete>Areas Only

To delete areas and all attached lines and keypoints (not shared with other areas):

Command(s):

ADELE

Main Menu>Preprocessor>-Modeling-Topo Repair>Delete>Areas and Below

6.2.3.4 Merging Gaps

Using the Automatic Merging Function

Saving the database allows you to "undo" the automatic merge operation if it provides undesirable results. If you find that the geometry is deformed by iterations at the higher tolerance settings, you can then reduce the maximum tolerance and try again. Remember, while you should try to fix as many gaps as possible at this stage, you can also repair gaps with the other modeling tools.

To automatically merge all gaps at the lowest possible tolerance:

Command(s):

GAPMERGE

Main Menu>Preprocessor>-Modeling-Topo Repair>-Mrg Model Gaps->Iterative

Using the Manual Merging Function

To merge gaps at set tolerance value:

Command(s):

GAPMERGE

Main Menu>Preprocessor>-Modeling-Topo Repair>-Mrg Model Gaps-By Tolerance

What If I Can't Merge All of the Gaps?

Exiting From Topology Repair

To exit from topology repair:

Command(s):

GAPFINISH

Main Menu>Preprocessor>-Modeling-Topo Repair>Finish

6.2.4 Using the Modeling Tools

• Use the geometry repair tools to fill large gaps (too large or ambiguous to automatically merge). To do this, you may need to create lines to complete continuous boundaries and then create areas within those boundaries. You can also detach unnecessary lines and areas from neighboring entities.
• Use the geometry simplification tools to eliminate disproportionately small geometric entities (such as very small lines or loops), extraneous features, or areas with disproportionate size in one dimension (sliver areas). Such entities can cause problems when meshing the model. The simplification tools work best when a volume is already created and it is recommended to complete volume creation operation before simplification.
• Use the geometry enhancement tools to create additional entities or enhancements. These tools were designed to work in conjunction with the Boolean tools and can be used to add through holes or enhance the model with geometric primitives. These tools are a subset of the standard, PREP7 geometry tools available in ANSYS.

6.2.4.1 Using the Geometry Repair Tools to Complete the Model

The general procedure you'll follow to complete a volume is

1. Find the holes or incomplete boundaries (gaps) in the model. In many cases, you can find these problems through a visual inspection of the model. To help you in finding gaps, the geometric repair tools include the same commands for plotting and listing unresolved lines that are in the topological repair tools. However, there is a minor difference between the way these commands function in geometry repair and in topology repair. The topology repair versions were designed to work with the merging tool, and therefore have preferences set through the GAPOPT command. The geometry repair versions of these commands have no such preference settings.

2. Approximate missing geometric entities. You can create a straight line between two existing keypoints to complete a boundary. You can than create an area within that boundary. Keep in mind that ANSYS always creates the minimum area defined by the boundary.

3. Create volumes using the completed areas.

Finding Incomplete Boundaries

To list open boundaries:

Command(s):

GAPLIST

Main Menu>Preprocessor>-Modeling-Geom Repair>-Lst Model Gaps-Open edges

To list all closed boundaries:

Command(s):

GAPLIST

Main Menu>Preprocessor>-Modeling-Geom Repair>-Lst Model Gaps-Closed edges

To plot all open boundaries (open edges plot in red):

Command(s):

GAPPLOT

Main Menu>Preprocessor>-Modeling-Geom Repair>-Plt Model Gaps- Open Edges

To plot all closed boundaries (closed edges plot in blue):

Command(s):

GAPPLOT

Main Menu>Preprocessor>-Modeling-Geom Repair>-Plt Model Gaps-Closed Edges

To plot both all open edges (red) and all closed edges (blue):

Command(s):

GAPPLOT

Main Menu>Preprocessor>-Modeling-Geom Repair>-Plt Model Gaps-Opn & Closed

Completing Boundaries

To create a line between two keypoints:

Command(s):

LNFILL

Main Menu>Preprocessor>-Modeling-Geom Repair>Fill Lines

Figure 6-2 An open boundary

Figure 6-2 shows a simple open boundary that can be closed by using the LNFILL command and selecting the two designated keypoints.

Completing Areas

To create an area from a set of lines:

Command(s):

ARFILL

Main Menu>Preprocessor>-Modeling-Geom Repair>Fill Areas

Detaching Non-manifold Entities

Figure 6-3 A Non-manifold Line Attached to an Area

To detach a non-manifold line from an area:

Command(s):

LNDETACH

Main Menu>Preprocessor>-Modeling-Geom Repair>Detach Lines

To delete a detached non-manifold line:

Command(s):

LDELE

Main Menu>Preprocessor>-Modeling-Delete>Lines Only

To delete a detached non-manifold line as well as all keypoints attached only to that line:

Command(s):

LDELE

Main Menu>Preprocessor>-Modeling-Delete>Lines and Below

Non-manifold areas are similar to non-manifold lines, and must be detached from their neighboring areas and then deleted.

Figure 6-4 A Non-manifold Area

To detach a non-manifold area:

Command(s):

ARDETACH

Main Menu>Preprocessor>-Modeling-Geometry Repair>Detach Areas

To delete a detached non-manifold area:

Command(s):

ADELE

Main Menu>Preprocessor>-Modeling-Delete>Areas Only

To delete a detached non-manifold area as well as all attached lines and keypoints (not shared with other areas):

Command(s):

ADELE

Main Menu>Preprocessor>-Modeling-Delete>Areas and Below

6.2.4.2 Using the Geometry Simplification Tools

Caution: Editing an entity with these tools removes any attached loads or boundary conditions. Therefore, you should simplify the model before attaching loads and boundary conditions.

Your model may contain

• Entities that are disproportionately small, such as small lines, loops, and areas.
• Entities that have disproportionate shapes, such as slivers and areas that are very long in one dimension.

The simplification tools were designed to eliminate such problem features. To help you identify these features, ANSYS provides functions to plot small areas, lines, and loops. Many such features can be found by a visual inspection of the model. You can also locate problems by meshing the model and then examining the error log and the resultant mesh.

The simplification tools only work on entities that have not been meshed. If you wish to apply these tools after meshing, you must first clear the mesh from the target entities.

Visual Inspection for Problem Features

Figure 6-5 Typical model entities that can cause meshing problems

Figure 6-6 shows the resultant mesh from the model. Note the rapid transition from large to small elements and the irregular mesh.

Figure 6-6 The mesh resulting from the features shown in Figure 6-5

The following section details the tools you can use to automatically locate small features, such as small lines and areas.

Locating Small Features

To locate small lines:

Command(s):

SLSPLOT

Main Menu>Preprocessor>-Modeling-Simplify>-Detect/Display-Small Lines

To locate small loops:

Command(s):

SLPPLOT

Main Menu>Preprocessor>-Modeling-Simplify>-Detect/Display-Small Loops

To locate small areas:

Command(s):

SARPLOT

Main Menu>Preprocessor>-Modeling-Simplify>-Detect/Display-Small Areas

The following figures show sample output from the various small feature plotting commands.

Figure 6-7 The output of the SARPLOT command showing an area that is disproportionately long in one dimension

Figure 6-8 The output of the SLSPLOT command showing small lines

Figure 6-9 A section of output from the SLPPLOT command showing several small loops

After locating problem entities, you can use the geometry simplification tools to remove those entities. The following sections outline techniques for removing such entities.

Merging Lines

Two lines can be merged together only if

• They are adjacent to each other.
• No other line is connected to them at the common point.

To merge lines into a single line:

Command(s):

LNMERGE

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Merge Lines

The example in Figure 6-10 shows a model (a) with lines that can be merged to form a much simpler model (b). For a model with such regular shapes and limited areas, you could merge all of the lines by using the LNMERGE, ALL command. However, you should normally merge lines "two-at-a-time."

Figure 6-10 The result of a line merging operation

Merging Adjacent Areas

Note-Area merge does not work for areas that contain internal loops (multiply-connected areas).

Figure 6-11 Maintaining a regular shape when merging areas

While you can merge more than two areas in one operation, you should only merge a pair of areas in each operation. This allows you to better maintain regular shapes and helps avoid problems during meshing. Area parameterization is dependent on the sequence in which the areas are merged. Merging two different sequences of the same set of areas may result in different area parameterizations resulting in a different mesh. If the merge operation would result in highly abnormal parameterization, the command will fail.

Note-Failure in area merge or failure in meshing as a result of poor area parameterization sometimes may be eliminated by deleting the area and recreating it using the ARFILL command.

To merge adjacent areas:

Command(s):

ARMERGE

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Merge Areas

Collapsing Lines

To collapse a line to a keypoint:

Command(s):

LNCOLLAPSE

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Collapse Lines

The example shown in Figure 6-12 shows the result of the LNCOLLAPSE command used to eliminate a small line and make the surrounding areas into more regular shapes. The figure shows only portions of the surrounding areas.

Figure 6-12 Use of the LNCOLLAPSE command

Collapsing Areas

Figure 6-13 A segment of a model showing a sequence of area collapse operations

When collapsing an area, you must first pick the area and then the line to which the area will collapse. As a rule of thumb, try to collapse an area to a longer (rather than shorter) line, and avoid collapsing an area with too many lines. It is sometimes advantageous to collapse the lines before collapsing the area. Also, area collapse does not work for areas with internal loops (multiply-connected areas).

To collapse an area

Command(s):

ARCOLLAPSE

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Collapse Areas

Splitting Lines

The most common use of this tool is to define a pair of new keypoints that can be used to split an area.

To split a line

Command(s):

LNSPLIT

Main Menu>Preprocessor>-Modeling->Simplify>-Toolkit->Split Lines

Splitting Areas

Caution: The command will allow you to create a split line that falls outside of the area and you should avoid creating such lines.

You should consider splitting areas in the following cases:

• To remove a "sliver area." To actually eliminate the sliver, you'll need to carry out additional steps (these steps are outlined in "Putting It All Together" toward the end of this chapter).
• To simplify a multi-sided area into a four-sided (regular geometry) area.

Command(s):

ARSPLIT

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Split Areas

Removing Area Loops

To remove an area loop:

Command(s):

ALPFILL

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Fill Loops

Removing Cavities and Bosses

Note-ANSYS will ignore this command if its result would cause excessive distortion or invalid model representations.

To remove a cavity or though-hole:

Command(s):

VCVFILL

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Fill Cavity

To remove a boss:

Command(s):

VCVFILL

Main Menu>Preprocessor>-Modeling-Simplify>-Toolkit-Remove Boss

Figure 6-14 Two through-holes removed by the VCVFILL command

Figure 6-15 A boss removed with the VCVFILL command

Putting It All Together

1. Create two keypoints by splitting lines in the area (b).

2. Create a new area containing only the sliver by splitting the original area at the two new keypoints (c).

3. Collapse the sliver area to a single line (d).

4. Collapse the remaining line from the sliver to a keypoint (e).

5. Collapse the lower line on the left side to a keypoint (f) to create a four-sided area (g).

This is just one example of how the simplification commands are used together. You'll find in most cases that planning what operations to use before removing a feature will make the job easier.

Figure 6-16 Various geometry tools often must be used to remove a feature

6.2.4.3 Reasons for Import Problems

• The CAD program may define entities in a manner that is not entirely conformant with a particular format.
• The CAD file may have been created in a way which is visually correct but causes problems for a finite element analysis tool (such as gaps, overlaps, etc., between areas).
• The CAD file may contain physical features that are difficult to mesh, such as "sliver" areas.

6.2.4.4 Limitations of the DEFAULT Option

• The option won't translate data such as dimensions, text, annotation entities, structure entities. Also, ANSYS ignores any IGES entities that the option doesn't recognize. However, the option will translate all IGES topological and geometric entities.
• ANSYS won't allow you to switch from the DEFAULT to the ALTERNATE option after importing the file, thus bottom-up model creation is not allowed.
• ANSYS won't allow you to export a model imported through the DEFAULT filter, that is, the IGESOUT and CDWRITE can't be used. If you must export the model, use the ALTERNATE option.
• ANSYS won't merge keypoints (NUMMRG, KP); merging is automatically done during the import operation.
• ANSYS won't concatenate lines and areas. However, area and line merging are possible.

6.2.5 Using the ALTERNATE Option

• ANSYS may be unable to import a model through the DEFAULT option and may advise you to try the ALTERNATE option.
• You may wish to export your model to an IGES file.
• You may wish to create new modeling entities on top of the imported model.

6.2.5.1 Importing IGES files for the ALTERNATE Option

Command(s):

IOPTN

Utility Menu>File>Import>IGES

• Select the Alternate option.

Command(s):

IGESIN

File picker dialog box that follows after setting IGES options.

Respond Yes when ANSYS asks if the IGES command should be executed.

6.2.5.2 Guidelines for Using the ALTERNATE Option

While Building the Model in the CAD System

• Observe ANSYS solid modeling procedures with regard to planning, symmetry, and the amount of detail needed for a finite element analysis. For example, for axisymmetric models, the ANSYS program requires that the global Y axis be the axis of rotation. Refer to Chapter 2, "Planning Your Approach."
• Avoid creating closed curves (that is, a line that starts and ends at the same point and closed surfaces (such as a surface that starts and ends at the same edge). ANSYS can't store closed curves or closed surfaces (it requires at least two keypoints). If a closed curve, closed surface, or "trimmed" closed surface-defined by IGES entities 120 and 144 or 128 and 144-is encountered while reading an IGES file, ANSYS will attempt to split it into two or more entities.
• As much as possible, write to the IGES file by data that the ANSYS program supports (see the description of the IOPTN command in the ANSYS Commands Reference).

While Writing the IGES File From the CAD Program

• Transfer only the portion of the geometry required for the analysis. A finite element analysis may not need as much detail as a CAD model requires.
• For trimmed surface transfer, include on the IGES file global XYZ data along with UV data.
• If the model to be analyzed is very large, use the CAD program's selection capabilities to create several IGES files, each containing a portion of the model. The ANSYS program will use the next available entity number as each file is read. You can then use the PREP7 merge feature (NUMMRG command or menu path Main Menu>Preprocessor>Numbering Ctrls>Merge Items) to merge coincident entities.
• Write the IGES file in ASCII format, with 80 characters per record.
• For the Pro/ENGINEER program, use these additional guidelines:
  • Set the Config.pro option "iges_out_trim_xyz" to "yes."
  • Set the accuracy to lE-6 and regenerate the model.

While Reading the IGES File into ANSYS:

• Pay attention to the messages issued by the ANSYS program. Warning messages give details of such things as IGES entities not transferred and the corresponding ANSYS entity numbers.
• If any IGES entities were not transferred, reconstruct them using ANSYS solid modeling commands. The ALTERNATE IGES filter is capable of reading in any rational B-spline curve entity (type 126), or rational B-spline surface entity (type 128) with a degree less than or equal to 20. Attempts to read in B-spline curve or surface entities of degree higher than 20 may result in error messages.
• Duplicate lines and keypoints are possible when transferring a model in from an IGES file. This often happens with CAD models due to the tolerances and practices that they were created with. You sometimes need to "clean up" these solid models with ANSYS commands that merge duplicate entities together (NUMMRG command or menu path Main Menu>Preprocessor>Numbering Ctrls>Merge Items).

Merging is done automatically when an IGES file is read into ANSYS [IGESIN] in AUX15. Default tolerances are used to determine if keypoints should be merged together into a single keypoint. Sometimes the default tolerances are not adequate and must be adjusted.

While Writing an IGES File from ANSYS:

• Set the system of units [/UNITS] before writing the IGES file. This information is captured on the IGES file and is read by many programs that read IGES files. (You cannot access the /UNITS command directly in the GUI.)
• Select all lower level solid modeling entities before writing the file (ALLSEL,BELOW,ALL or menu path Utility Menu>Select>Everything Below).
• If you wish to write out only a portion of your model, select only those entities to be written (that is, areas) and all corresponding lower level entities (lines and keypoints). Then unselect any higher level entities (volumes) before writing the file.

6.2.6 Using the Remaining Modeling Commands

Go to the beginning of this chapter