plunge roughing

[HEAVY METAL]

Hello

I am trying out the plunge rough toolpath.What I

want do do is rough a 8.189 dia thru from solid.I plan to drill an entry hole and start from there and step around the outside following the circle then having a slug which will fall thru.Is this possible to do with plunge rough option? Has anyone done something similar?The material is h13

I am open for suggestions.

 

thanks Heavy

[jeff]

How thick is the part?

have you tried "contour/ramp"?

I haven't used the plunge rough yet,it seems like it would take too long.

[P_Scott]

Heavy Metal,

 

Are you asking about Surface-Rough-Plunge toolpath? If so, this will not cut around a "slug". The rough plunge is designed to remove a large amount of material from a cavity by either "drilling" the material or helixing into it, using a grid pattern of points. As Jeff said, using a 2D Contour-Ramp may produce better results. You can also produce a toolpath to drill the start hole for the contour AFTER the contour has already been made. This start hole toolpath is part of the Circle Toolpaths menu in Mcam V9. HTH

[steve f]

HEAVY METAL,

 

I understand what you're trying to do and have done the same with the exception that instead of plunge roughing the slug out I just drilled it out. The problem you might run into if you create a slot around the entire circumference of the slug is that it'll fall through or shift when your tool breaks through the last bit of material and probably destroy your cutter in the process. Try making a pattern of circles (the same dia. as your drill) around the inside of the hole geometery so that all the circles are touching but not overlapping. Drilling will leave a thin web between the holes since the material is pushed over slightly and your slug won't fall through when you get to the last hole. The last step just requires a little "percusive maintenance" with the biggest dead blow hammer you can find to knock that slug out when drilling is complete. This has worked for me on a number of occasions.

 

STeve

[Roger Peterson]

Heavy, yes you can and it works quite well. In the plunge rough toolpath you can do zigzag or nci. Before you do your plunge roughing toolpath do a contour toolpath around whatever shape you want to plunge around. When doing this use the same tool as your plunge rough toolpath and leave some x,y stock to leave to make sure your plunging doesn't gouge the wall. What I do to keep the slug from falling or tipping and breaking the tool is not go all the way through the part by using the cut depths. And as Steve said a nice big hammer and metal chisel will get your slug out from the bottom. This also works with pocketing routines for die work.

 

 

hope this helps,

[HEAVY METAL]

Thanks Roger for the idea I will give this a try and let you know.Thanks also to everyones input.There are some good suggestions.Now I am going to do a little experimenting

 

have a nice afternoon heavy

[HEAVY METAL]

Roger i tried your idea.I made a 2d profile tool path of the dia. Then used plunge rough with that path's nci but the toolpath is wanting to jump around the outside of the profile and is not completely cutting the hole profile to produce the slug.Do I have some parameters set wrong?I also gace zig -zag option a shot but it was even worse

 

 

thanks heavy

[Roger Peterson]

Heavy, one thing I see I didn't mention is that you will have to create a flat boundary surface at the bottom of you hole. If there is no surface directly below the where your tool cuts there is nothing to project the nci path onto. Other than that I am not sure without looking at the file.

 

 

Heavy, in your 2d contour you need to compensate for the tool diameter plus some stock to leave to inside of the boundary of the hole. Did you do this? If you have cutter comp set to off it will do strange things.

 

 

Let us know,

 

[ 04-16-2003, 12:10 PM: Message edited by: Roger ]

[HEAVY METAL]

HI Roger I will try making the flat bottom surface.This something I left out.

 

thanks heavy

[HEAVY METAL]

Hi Roger your suggestion was right on the money.I am getting the toolpath that I want but it wants to take multiple passes around the inside and it looks like it is just cutting air on these passes.I have my cut depths set where the first pass is cutting just shy of breaking thru then it looks like it is just repeating the same path over and over

 

 

thanks heavy

[McRae]

Heavy,

 

What about just using a drill toolpath? Set a bolt circle at the diameter you wnt to plunge out minus the diameter of the tool. Now take that diamter and multiply by pi (3.1415) and find the circumfrence. Divide the circumfrence by the tool diamter and select the next whole number(round up). Divide this result by the amount you want to overlap (ie 14/.75) and then this is the number of holes to put on that bolt circle. Program the depths - and post the code.

[Roger Peterson]

Heavy, do you have multiple passes or depth cuts in the 2d contour operation. This is probably why. I'm glad this is working out. One of the nice things about this toolpath is that you can bring everything down to a height and then step it down again. I have used the drilling method but depending on how deep you go you have a long way bring up the chips.

 

 

Let us know Heavy,

[HEAVY METAL]

You da man Roger!!!!!!!

The depth of cuts in the 2d contour was the problem.Thanks for your help I learned alot in a very short time. Also, thanks everbody for their opinions.Some great ideas that I might be able to use down the road.

thanks Heavy

[Roger Peterson]

No problem, you have to get lucky once in a while.

 

 

Let us know how much fun you had pounding the slug out...

[Kevin Goddard]

I just tried doing the surface-rough-plunge op and when I get to the select drive surface I can not select anything. I am new to surfacing so please bear with me. I created a 8" c'bore 2"deep in a 10" body in solids. I assumed from your post about having a surface at the bottom of the hole that a c'bore would work. I am not sure what I am missing (the big picture maybe). Could you please walk me through this if you get the time. Mill & Lathe V9.0 SP1 Level 3 Solids. Thanks....Kevin

[HEAVY METAL]

Hi Kevin

The first thing you will need to do id make a 2d contour toolpath for the c-bore dia.You will use this paths nci file for your surface rough plunge path.In the plung parameters select nci the select that 2d-c-bore operation.You should only have to select the bottom surface of the c-bore.I,m not sure why you are having trouble selecting this surface without seeing the file.You can post file to ftp or e-mail it to me and I will have a look.

 

 

see ya Heavy