How do you change the spindle speed in the middle of a tool path?

I was recently wondering if there was a way to change the machining speed in the middle of a tool path in CATIA's advanced machining workbench. I have a part that we want to enter slowly, proceed along a surface, and then change to the regular machining speed. Breaking the tool path into two operations is NOT possible in this situation. One solution, though not ideal, is to use the Toolpath Editor and inset SPINDL speed changing statements at the desired point using the PP Word Modification.

This option will lock the toolpath so you must make sure you have finalized your machining operation. If you unlock and regenerate the MO then you will lose all of the toolpath modifications, which makes this solution not the best one, in my opinion, but the only one I've discovered which works thus far. Any other solutions?

CATIA NC Machining Reverse Motion Fix

I am machining some parts in CATIA V5 R18 and if I zoom in on the vectors in wire-frame mode I am noticing areas where the tool is reversing a fraction of a millimeter, which has become an issue. I need to eliminate all of these reverse motions. My two major concerns are:

1. What is the easiest way to detect these reverse motions? Currently, I have to zoom in really close on the vectors, the only way I know how to see them in CATIA, which is a pain.
2. How do you avoid this reverse motion? What's the best way to fix them?

The answer to question number one is unfortunately there is no other way in CATIA to detect these tiny reverse motions. If you have some sort of post-processor that will usually pinpoint problem areas but if you don't have access to a post then you're out of luck. As far as concern number two, my guess is the surfaces are crap (especially if they are not native CATIA data and imported from some other system). You can try to rebuild them to get better results. Often times, I will delete the two axial moves using the toolpath editor. Then, I will select the icon to connect the path, select one of the high-lit points, and enter .000 as the value. This way, you will get a direct connection in machine feed. It's kind of weird, but if I want a Rapid connection, I will enter .1 as the value.

Also, sometimes, as in the example, you would end up with a small zig-zag motion. In that case, I will often delete a point if available or move a point along the direction before "connecting" it. As always, toolpath editor is last resort but I'll use it rather than spend a bunch of time fighting surfaces and machining operations. I always note in my programming log, any locked toolpaths, why, when, and what type of edit was made. It's good to keep a log using Excel for whenever you have to make "manual" edits of any sort.

How do you write code for Catia’s Expert Check Editor?

I've been trying to use KBE (Knowledge Based Engineering) to try and automate a checking procedure on an NC machining process in CATIA V5. The customer requirement is for all cuts to be in the climb direction, not conventional. Using the expert check editor I can implement a checking system to easily make sure all machining operations are compliant with this requirement. Syntax is the trickiest part of the KWE language, so pay close attention to every key stroke you make when programming. Here are the steps:

Knowledgeware>Knowledge Expert Workbench>Expert Check Editor

Be sure to select the KWE Advanced Language from the pull down menu. Now enter the following code:

For All entry: FX:Mfg5AxisCurveMachining; CX:Mfg5AxisFlankContouring

Body entry: /* only interested in multi axis curve operations containing the word "Rough" */

if FX->Name()->Search("Rough")>=0

{

    if FX.MfgDirectionOfCut=="MfgClimb"

    {

        ThisCheck->AddTupleSucceeded (FX)

    }

    else

    {

        ThisCheck->AddTupleFailed (FX)

    }

}

 

/* only interested in multi axis curve operations containing the word "Finish" */

 

if FX->Name()->Search("Finish")>=0

{

    if FX.MfgDirectionOfCut=="MfgClimb"

    {

        ThisCheck->AddTupleSucceeded (FX)

    }

    else

    {

        ThisCheck->AddTupleFailed (FX)

    }

}

 

/* only interested in multi axis FLANK CONTOURING operations containing the word "Chamfer" */

 

if CX->Name()->Search("Chamfer")>=0

{

    if CX.MfgDirectionOfCut=="MfgClimb"

    {

        ThisCheck->AddTupleSucceeded (CX)

    }

    else

    {

        ThisCheck->AddTupleFailed (CX)

    }

}

Catia NC Programming using Check Editor Knowledge Based Engineering

I use the check editor in Catia V5 to improve the quality of NC machining process files. All of my chamfer cuts on this particular part need to have a Tanto Fan axis. I use the code below:

`Far Side Chamfer 1\MfgParameter.5\Tool axis strategy` == "MfgTantoFan" AND
`Far Side Chamfer 2\MfgParameter.5\Tool axis strategy` == "MfgTantoFan" AND
`Near Side Chamfer 1\MfgParameter.5\Tool axis strategy`== "MfgTantoFan" AND
`Near Side Chamfer 2\MfgParameter.5\Tool axis strategy` == "MfgTantoFan" AND
`Near Side Chamfer 3\MfgParameter.5\Tool axis strategy` == "MfgTantoFan"

All of the machining operations in my part need to be climb cut. Therefore, I used this code in the Catia check editor to let me know if it somehow gets changed by accident.

`Rough Far Side.1\MfgParameter.5\Direction of cut` == "MfgClimb" AND
`Rough Far Side.2\MfgParameter.5\Direction of cut` == "MfgClimb"

Keep in mind you can't just use a plain old equals sign, you need to use the double equals. Also, it took me awhile to figure out the correct syntax for  "MfgClimb". I tried "Climb" and MfgClimb unsuccessfully before stumbling upon the successful solution.

I use a parameter to control the depth periphery (depth of cut) and the distance on the rough profile from the tool to the part. Here are the simple formulas for the check editor.

Depth_Periphery == -2mm AND RoughProfile == 1.5mm

/*Check created by Me 7/12/2010*/

CATSettings Pointers for CATIA Users

I'm starting to realize deleting the CATSettings fixes a whole bunch of strange issue in CATIA.

 

Recently had this problem in CATIA NC workbench:  cannot pick the start/stop points in Multi-Axis Curve Machining.  This only happens with his log-in on his computer; using his log-in on another computer works fine.  The points, in the machining operation window (where you pick other driving geometry) are shown as solid black dots.  Is this a Tools -> Options issue?  Un/Re-installing CATIA doesn't fix this either. V5R18SP7.  Everything else (as far as we can see) works fine.  Any ideas?

CATSetttings is probably the biggest quirk in CATIA V5. I made a screenshot of all my Tools/Options and anytime we go to another revision I recreate my CATSettings. Like many other people, I learned the hard way. Anytime something is acting strangely it usually ends up being the CATSettings.

A few other CATSettings pointers on this. Do not use the same settings folder for multiple versions (R18/R19), keep a back up copy of a clean start - they will get corrupt from time to time. When unpredictable things happen - example your picking issue, replace your settings with clean set. Re-installing Catia does not clean up your setttings directory. You can find your directory in C:\Documents and Settings\USER NAME\Application Data\DassaultSystemes.
In there I would create CATSettingsR18 and CATSettingsR19, to do this you need to modify in the Environment Editor the path in variable CATUserSettingsPath.

What kinds of analysis and collison detection errors can Vericut perform?

I began learning Vericut a few weeks ago. Vericut is an analysis program, the goal of which is to detect errors in NC programming. The types of errors that Vericut detects are as follows:

Rapid cut into material

Holder collision

Fixture collision

Shank rubs on the part

Tool wrong size

Incorrect tool length or diameter compensation

Cuts exceeding tool capability

Reamer/tap collision

Thread size/shape

Boring bar orientation

Gouges

Excess material

Machine collision

Machine over travel

Spindle off

Spindle wrong direction

Coolant on/off

Table clamp on/off

Incorrect feed rate value/mode

Probe collision

Wrong syntax