Home  > Collaboration > Discussion Forum > Active Discussions

Welcome to the COE Discussion Forum! 

 

To participate in the discussion forum, you must be logged in to the website.  If you forget your login information, please contact COE Headquarters at coe@coe.org or (800) 263-2255.

If you are new to the COE Discussion Forum and would like to participate, please register.
Forum Highlight: CATIA V6

 

Get Answers to Your V6 Questions
Dassault Systèmes answers user questions about CATIA V6.  Discuss these answers and propose new questions with end users from around the world in the CATIA V6 Forum.

COE DISCUSSION FORUM
Forums > COE Forums > MFG
Subject: wheel cutter/ normal to ps

You are not authorized to post a reply.   
Author Messages
LUPAC

12 Sep 2008 01:35 PM

wow, what a mess! does anybody know if there is a trick to flank contouring a wheel normal to part surface? i have the machining tolerance down to .001. it took about 10 minutes to calculate the path. please check out the attached pic





BFELSHER

12 Sep 2008 02:03 PM

Hmmm....shouldn't take that long. Are you using a "T-slot" cutter? I'd just use a regular endmill for calculation purposes.

I've posted before, but there MAFC ignores a contact height taller than the CUTTING (FLUTE) length of the tool. MAFC comes from NCL, so I understand the reasoning. So...it works a lot better if you create a tool that has cutting flute the entire length of the tool.

In other words, don't use a wheel cutter or even an endmill with just .250 or so OAL, Cut Length, and Length. Try using an endmill in Catia that has a cutting length more than the wall height. This will give you the best fastest calculation. Then, in Vericut- use the correct tool description/model. For MAFC, I just about always if I'm using a 1" endmill for instance have a tool 1" Diameter, 2" OAL, and 2" flute. This will give a clean toolpath calculated fast. Think APT.

It's not as if the top of the wheelcutter needs to be considered for calculation purposes.  It's just a visual thing.  If you need to see the visual in Catia (which I always like to see- especially for saving CGR's and subsequent path verification), lie to Catia about the tool, and then use a "user representation" for video replay.
Bryan Felsher
True Precision
LUPAC

12 Sep 2008 03:22 PM
thanks bryan,
the cutter described in catia is a 2.0" dia. w/.12 rad 1" flute length. in vericut i define a wheel .500 wide w/.12 rad both sides.
BFELSHER

12 Sep 2008 03:53 PM
Well, it seems you're doing it pretty much exactly how I do it...don't know what to say. When I have MAFC paths that take a long time to compute, most often it's because of the way the surface is built. Many times, I've rebuilt surfaces. I'm sure you know all about that! I know you know this- I'm just writing for those who don't...Anyways, if you can build surfaces as simple as possible (1st choice Ruled- 2nd choice Trimmed to a flat planar boundary), everything works much better. Obviously this isn't always possible. So I try and use Extrude and Multi-curve surfaces (I think it's called?). Swept surfaces don't work very well because most of the MO's usually need to recognize individual patches. Anyone remember the good old days of COONS surfaces? That was a pain in the butt to construct!

Anyways, I don't see what you're doing different than I would. Maybe try rebuilding surfaces. Sometimes just untrimming surfaces does the trick. Or cheating and creating planes tangent to a surface that is 99% planar.

Sorry man, I'm not sure why it's taking so long to compute. It could be a parameter setting, max-disc step value too small, maybe it doesn't like the cut distance setting. Changing that bigger or smaller often times can have a positive affect. I feel your pain, especially if there's a lot of paths to create.
Bryan Felsher
True Precision
SAMARINDER


12 Sep 2008 07:59 PM
I've posted before, but there MAFC ignores a contact height taller than the CUTTING (FLUTE) length of the tool. MAFC comes from NCL, so I understand the reasoning. So...it works a lot better if you create a tool that has cutting flute the entire length of the tool.


Try using an endmill in Catia that has a cutting length more than the wall height. This will give you the best fastest calculation. Then, in Vericut- use the correct tool description/model. For MAFC, I just about always if I'm using a 1" endmill for instance have a tool 1" Diameter, 2" OAL, and 2" flute. This will give a clean toolpath calculated fast. Think APT.


You can use check box on Tool Axis tab-"Control fanning using tool parameter" or in other words "fake length just to control fanning". "Contact height" in other words "dont gouge the wall with given flute length of the cutter"
Samarinder Singh
NC-Programmer/Tool Designer
LUPAC

15 Sep 2008 08:40 AM

thanks for the replies,

is there anyway of telling catia the max distance between points that it outputs? if you see the result of what ncl can do (see pic) there must be a way for catia to do the same thing i would think. i already have the machining tolerance down to .001". and i was exagerating, it takes less than 1 minute to process.





BFELSHER

15 Sep 2008 10:00 AM
Set Max Discretization step or Max Angle step or both. The tolerance works more like INTOL/OUTTOL so won't neccesarily make more points output. To ensure linearization on rotary head 5-axis, you need to output more points especially where there are big angle changes.
Bryan Felsher
True Precision
LUPAC

15 Sep 2008 12:24 PM
thanks for the help,
i was able to change the max discretization to .030 and max angle to 1 degree and the results were alot better.
BFELSHER

15 Sep 2008 12:44 PM
Try leaving max step at 400 inches and setting the max angle to a really small number maybe .5 degrees or less. I have good results with that.
Bryan Felsher
True Precision
You are not authorized to post a reply.
Forums > COE Forums > MFG > wheel cutter/ normal to ps


ActiveForums 3.6

    

401 North Michigan Avenue, Chicago, IL 60611-4267 | (312) 321-5153 | (800) COE-CALL (U.S.)