Build Thread- High Speed Pocketing in BobCAD ?

[gn3dr]

Originally Posted by The One If your line 64 does not have the z_f variable in the line then it should definitely be added. If your using a custom post processor, one you have already modified, then you will want to download the post from the web and use a diff tool to see what the differences are. There are some additional lines in the posts for the recent release, build 1326. They pertain, mainly, to the header needed for the Predator Editor to do a backplot. Regards

Thanks The One
I had not modified my post and I had download build 1326. My post didn't have the z_f part in it. The post processsors on the support site also didn't have it.
So my post line 64 now looks like
64. Arc move.
n,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate

Should I also add in g_arc_plane?
Or better yet - where could I download the standard Mach 3 Metric Post for High speed pocketing?

[The One]

Those posts should have all been updated. Do you have the automatic tool changer? I can post it here for you.

I have talked to Brain at Mach3 and the post that I have on my system is approved for the machines without the ATC.

Regards

[gn3dr]

Originally Posted by The One Those posts should have all been updated. Do you have the automatic tool changer? I can post it here for you. I have talked to Brain at Mach3 and the post that I have on my system is approved for the machines without the ATC. Regards

Hi
That would be great if I could post it here for me. I don't have the ATC.
Regards

[laserkey]

Just make sure you are getting x,y&z in a g02 or g03 move because that was my problem . If not it will drop into the material instead of feeding into it .
I want to say that my post was cleaned up and everything seems to be fine.
The response was very quick as i do believe it was just foresite.
The tool path is great if you have a high spindle speed and can handle light cuts at super fast feeds . We are running at 300 ipm. but it does not always run that though. Which makes my cutting time down to at least half.
The only thing is if i pick two hole ops. and tell them one is 54 and one 55
it makes them both what ever the fist one is . So im going to have someone look at this. I am running on haas machines also . so if you would like this post vfmill.mlpt please reply.

[robrea]

I recently purchased the HSP package. I am having trouble getting the circular moves to also drop in z. The path looks good in Predator. If I post the code I get only z moves in the straight line moves.

I played around with the post using the recommendations somewhere else on this post. It didn't seem to help.

Am I missing something?

Anybody else using the HSP?

Thanks,

Robert

[laserkey]

open your post in the note pad and look at line 64.
This is what it should look like.
64. Arc move.
n,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate


once you do this just click on file and then click on the save button ,not the save as button.

[robrea]

Laserkey,

I tried editing the post. I was carefull to cut an paste exactly as you have shown. Still, in predator the path looks good. The post however doesn't show Z movement in circular paths.

I made a tech request to Bobcad for assistance.

Otherwise the path seems to work well. The movements are full arcs instead of broken line segments. Should cut very fast.

I'll let the forum know as soon as I have some real pockets to cut.

Robert

[nlh]

Robert,

Based on my limited experience (V23 demo, and volumill's 14 day website trial), the material entry is not a true helical path. More of a rectange, picture the cutter moving in a linear path, then performing a 180deg. arc, a linear path in the opposite direction and then another 180. The z moves should be in the linear portions, not the arcs. Which is why it looks like it's working correctly in predator, but examination of the code makes one think otherwise. It took me a little bit to catch this one myself. Hope this helps.

Nate

[The One]

Robert,

More than likely, there is more than one line 64 in your post. This is a case of "the last one wins". Look at the very bottom of the post in a text editor. You should see an additional line down there that needs to be changed or removed. I would suggest removing it if it is there and if you have already modified the line 64 that is in the right location.

Regards

[robrea]

Thanks everyone,

There were two line 64's. After editing the second one HSP does spiral down in the G03 lines and continues at the same rate in the G01 lines. This way the descent angle doesn't violate the ramp rate the endmill is capable of.

I am anxious to practice on some pockets and compare cycle times and endmill life.

As nlh suggested, the ramp is sort of a rectangle. But, I get G03 x,y,z and G01 x,y,z drops. This is the way I understood the path to work.

I'll post some paths and reviews as soon as I can.

Thanks again,

Robert

[nlh]

Glad to hear you have it working Rob,

Will be interested to hear how it works out when cutting material. Keep us posted. BTW, what machine (make, model, control) will you be using?

Nate

[robrea]

nlh,

I work several jobs. Primarily I am plant engineering, using mostly Mori Sieki mills and lathes with Fanuc 0 and 10 controls. The part time shop has a variety of machines. Ranging from older Mazaks to latest with Fanuc 21i. I mostly program the fanuc based machines with subs and macros. They have me come in for these 'special needs' programs using macro variables, adjusting the cutter comp path sequentially as we jig grind, etc.

This HSP will save me a lot of work.

I've read the forum for years, I am going to try to be more proactive when people need help. I see a large variety of problems/solutions.

Thanks again,

Robert