5-Axis Gouging

[Colin Gilchrist]

The last one I did was proprietary, but I can make one that is similar.

 

The first thing that I had to wrap my head around was that the "Triangular Mesh" Toolpath is basically just "surface roughing", that ignores the surface normals and only worries about the contact point of the tool on the surface.

 

All the other surface 5X toolpaths make use of the surface normal in some way for the Toolpath calculation. The Triangular Mesh toolpaths are just "surface roughing" and "surface finishing" with a different name.

 

You'll see under the Cut Parameters that there are many different strategies that offer similar options to other surface paths in Mastercam. The "Rough" option is the only one that offers Adaptive Clearing. This is a 3X style path, so you need to pick a direction, and you can use a Tool Plane to do that. You get to take advantage of all the linking options though, so you get great control.

 

The path is all Vector Based, which means you get a ton of code, but it's much easier to convert to a 5X path for this reason.

[Reko]

Hey Tom,

 

Are you using the Adaptive Clearing with the Triangle Mesh toolpaths?

 

Lolz!

 

Not yet... but give me time... and keep those suggestions coming... that sounds like full control with your hand on the throttle!

[Reko]

I would suggest the IHS Handbook Volume 3 as well, it breaks down the functions of each of the utilities in the multiaxis toolpaths with visual references.

 

CJep... I'm not seeing that anywhere... link?

[crazy^millman]

Colin You have mail.

[gcode]

Hey Tom,

 

Are you using the Adaptive Clearing with the Triangle Mesh toolpaths? That lets you create Dynamic style Toolpath motion with the Advanced Multi-axis Toolpaths. I've been generating some awesome paths with it lately. I then take the Adaptive Path, and use the 3X to 5X Toolpath to get the tool axis control I need. The end result is a full 5X path with Dynamic motion, and all the collision control you need. I especially love being able to set a Zig-Zag cut pattern with the Adaptive Clearing. With Zig-Zag, you can independently set the Climb engagement and the Conventional engagement as a percentage of the max step over. This means your tool never cuts air as it cleans out the corners of the material. I really like using 100% of the step over for climbing, and 35% for the conventional cuts. It lets me squeeze out a little quicker cycle time...

 

No, but I'd sure like to see a sample of this

[Colin Gilchrist]

Tom/Ron,

 

I'll see what I can do to put together an example...

 

Ron, I got your message...

[Nils N]

Colin, I'd like to see that too. I'm have some 5 axis projects I'd like to have better control on.

Oh and hows it going on the other coast?

[Colin Gilchrist]

Hi Nils,

 

I'll post something up when I get a good sample.

 

Living in Connecticut is great. I miss Seattle sometimes, but I got married in May, and couldn't be happier. I hope all is well with you and your shop.

 

Regards,

 

Colin

 

 

[Maclaw]

I don't see a "max angle increment" but my angle increment is set to 3, which is the default.

 

Acording to the specs (from haascnc.com website) Your trunnion has a max speed in both axis (A-tilt and B-rotary) of 50deg/s.

 

If You were incrementing the angle in each block by 3 deg and Your feed was at 999.9 inverse time, then You made Your trunnion axes travel at this speed:

 

3deg / (60/999.9) = 49.95 deg/s -> the TOP PHYSICAL SPEED LIMIT of Your trunnion.

 

Maybe on relatively "flat" areas it handled the job, but at those 4 points where rotary travel had to be significantly large in comparison to the actual movement of the tool on the surface - it lost sync and gouged the part. Look at Your NC code in the 4 "tough" areas - maybe the block-to-block swing was even larger at those 4 points - then the max speed was for sure even further more exceeded... It might be that You asked your poor trunnion to "rock and roll" faster than it physically could....

 

You then stepped down to F150 inverse and You completed the job with no gouges. But this speed on the other hand was very sssslow at overall and increased Your cycle by 6+ times... I don't blame You complainig there - after all time is money :-)

 

Maybe the job would be ok if You went down by half the speed (You'd have about 2 safety factor from the max speed of your trunnion) - I don't know. But I am verey curious about Your NC-code fragment in the areas of the "tough" cuts.

 

I also agree with Aaron and the other Guys that increasing the amount of vectors would be definetely a plus.

 

Guys - I dont think that Haas ever said that the trunnion speed limit is 1000, 4000, 40000, 60000 or whatever else inverse time feed. In my opinion this is for the user to figure out because it depends on the angle increments you ask it to take in one block. You have to calculate the max feed inverse time you want to make it move by - taking into account the max speed of your table. Correct me if I'm wrong (it's late here and I might talk bull*) :-)

 

I am having a similar issue I'm working on - only in 4-axis with HRT160 - if I have something wise to tell You I will :-). An additional thing I had to do is change parameter 104 for the A-axis ("in position limit" or something like that). It was set originally to 4000 and I changed it to 20000 (!!!) because otherwise at about 4 angle increments (block to block) and at inverse feeds greater than 200 on a CYLINDER (don't laugh - I was jus testing :-))) my table was jerking like a wild horse. That's a separate thread I started ("Haas rotary parameters") - don't want to get asked out by the Moderator for not staying with this subject :-)

 

Reko - good luck and give us some info on Your further thoughts.

[Reko]

Mac... originally, I started out at 3 degrees, then, based on suggestions I closed it at several different increments all the way down to .5 degrees.

 

No matter the angle increment, it still out kicked out F999.9 and still gouged the part... which makes sense because whether I machine a 1" line in a single block, or I break it into a thousand line segments and machine it at the same feed rate.. I will still reach the end point in the same time frame... right?

 

The answer for me, was to set the feed at 150.

 

I still don't know the answer to the question... how do I see something like this coming without scraping a part?

 

In the future, I will look for big swings and program accordingly, but I am still not certain how to force the post to slow the "F" when the A and B axis makes big swings.

 

I intend on looking to some of the more advanced toolpaths in the future to see if I can get more feed rate control in the area's I want. That is likely my answer.

[CJep]

CJep... I'm not seeing that anywhere... link?

 

It's here in the book store.

 

http://www.emastercam.com/board/index.php?app=nexus&module=payments&cat=135

[Reko]

It's here in the book store.

 

http://www.emasterca...ayments&cat=135

 

Thank you.

[Nils N]

Colin CONGRATULATION on getting married!! Sounds like things are going your way back there.

May all your ups and downs be between the sheet1!! Best of wishes to you and your bride

[Colin Gilchrist]

 

On 11/6/2013 at 1:27 PM, Nils N said:

Colin CONGRATULATION on getting married!! Sounds like things are going your way back there.

May all your ups and downs be between the sheet1!! Best of wishes to you and your bride

I'm about 8 years too late Nils, but thank you!