DYNAMIC & RADII INTO VEIN

[CNCZACK]

I've got this part I've been trying to program but I continue to get stuck on this one. Below is the file.

Were working on getting more memory to the machine that this will run on (currently only holds 75KB at a time, so I'm having to work around that and fight with using import nci ). Work holding is something were working around as well with this (I think were going to use a chuck and have the operator move the clamps as it gets to a different section).  Is there a way dynamic milling can be sectioned up to have both of these problems solved without it being a mess with crashes? Also with the radius, I can get it in there but you can see in the corners it leaves a radius, and I'm not sure what toolpath would work best to getting into the corner and flow up to the veins..

any and all suggestions on this one. 

 

 

mill internet.mcam

[#Rekd™]

Look at using a Scallop toolpath with a boundary chain to limit the tool. Use a small diameter ball nose to limit the corner rads.

 

[JParis]

Morph between 2 curves will be your friend here...

BUT......you have program size issues....

I don't have time this morning but I might draw lines along those vanes and use a project toolpath to rough it out...you should have some better filter options that way.

[CNCZACK]

22 minutes ago, #Rekd™ said:

Look at using a Scallop toolpath with a boundary chain to limit the tool. Use a small diameter ball nose to limit the corner rads.

 

I believe I dont have it unlocked or im using it wrong. I can select only one surface, then it tells me its" incompatible with current mastercam product or level"

19 minutes ago, JParis said:

Morph between 2 curves will be your friend here...

BUT......you have program size issues....

I don't have time this morning but I might draw lines along those vanes and use a project toolpath to rough it out...you should have some better filter options that way.

I dont have that available either 

[#Rekd™]

15 minutes ago, JParis said:

Morph between 2 curves will be your friend here...

Much better solution than mine, I didn't think they had a muti-axis license!

[crazy^millman]

Does the part have real sharp corners? I have done parts like these over the years and they never have a real sharp internal corner. What is the max radius allowed? Grab a Bull endmill with that Radius and look at using it. What kind of machine is this? I see 4 Axis defined in the File so with that you are limited in your choices of toolpaths. I might old school this and just do are Surface Finish Contour from the plane you have defined and call it a day. Break each depth section into the machine size limits and have tapes A-Z, AA-AZ, BA-BZ and such until you have made a complete program. Right click on each section and use the rename NCI to make them all different program names for posting and done. I normally make Toolpath groups for each tool or tape, but sounds like people could care less about organization and just get it done. What is the profile tolerance on the 5" Radius area or the .5" radius Area? What is the surface finish requirement?

Tape A to Tape Z

Tape AA to Tape AZ

Tape BA to Tape BZ

Right there is 76 Tape names and easy for anyone to follow and track and they run them on the machine.

[CNCZACK]

21 minutes ago, crazy^millman said:

Does the part have real sharp corners? I have done parts like these over the years and they never have a real sharp internal corner. What is the max radius allowed? Grab a Bull endmill with that Radius and look at using it. What kind of machine is this? I see 4 Axis defined in the File so with that you are limited in your choices of toolpaths. I might old school this and just do are Surface Finish Contour from the plane you have defined and call it a day. Break each depth section into the machine size limits and have tapes A-Z, AA-AZ, BA-BZ and such until you have made a complete program. Right click on each section and use the rename NCI to make them all different program names for posting and done. I normally make Toolpath groups for each tool or tape, but sounds like people could care less about organization and just get it done. What is the profile tolerance on the 5" Radius area or the .5" radius Area? What is the surface finish requirement?

Tape A to Tape Z

Tape AA to Tape AZ

Tape BA to Tape BZ

Right there is 76 Tape names and easy for anyone to follow and track and they run them on the machine.

I dont have a sample part but from what I  gather the corners dont have to be incredibly sharp.

Im thinking max radius would be .125R.

This is a V-center 105 with an A axis that does not work anymore.

What do you mean by breaking each "depth section", last time I imported nci I just did the max memory limit because I quickly got into 10 programs lol. 

The .5" area is not toleranced on print so we go with .015" one the tolerance and a 125 finish all over the part 

 

[crazy^millman]

2 hours ago, CNCZACK said:

I dont have a sample part but from what I  gather the corners dont have to be incredibly sharp.

Im thinking max radius would be .125R.

This is a V-center 105 with an A axis that does not work anymore.

What do you mean by breaking each "depth section", last time I imported nci I just did the max memory limit because I quickly got into 10 programs lol. 

The .5" area is not toleranced on print so we go with .015" one the tolerance and a 125 finish all over the part 

 

Each toolpath has depth settings in them to decide a area of place you want to cut. Part is 2.000 tall and cutting from .0 to -.2 creates 1000 kb of code. Then you make one toolpath that cuts everything and you then copy and paste it 10 times. Then in each toolpath you change the depth settings to cut just that section of the part in that. Now if .2 of area is too much then just change the settings to limit how is being cut and then just track the correct over lap to get what you need. Go to a 1/4 ball endmill for the finish you need.

[CNCZACK]

2 minutes ago, crazy^millman said:

Each toolpath has depth settings in them to decide a area of place you want to cut. Part is 2.000 tall and cutting from .0 to -.2 creates 1000 kb of code. Then you make one toolpath that cuts everything and you then copy and paste it 10 times. Then in each toolpath you change the depth settings to cut just that section of the part in that. Now if .2 of area is too much then just change the settings to limit how is being cut and then just track the correct over lap to get what you need. Go to a 1/4 ball endmill for the finish you need.

thats a good option, ill give it a shot! 

[crazy^millman]

14 minutes ago, CNCZACK said:

thats a good option, ill give it a shot! 

Yes very powerful process and helpful with older machines with limited memory. I use it with certain customers.

[AMCNitro]

Trying to upload and it wont let me. 

First, use only the 3/8 tool and do a dynamic with the big circle set as AIR, you can do it in one shot with one tool, forget the 1/2 endmill. -

To do the radius use a flat endmill with the Flow Line, it will leave a sharp corner.  It works, I've done it dozens of time.

One more thing, use filters.  Don't forget the filters.  Did I mention filters?

Don't be afraid to do surfacing with flat endmills.

IF I could upload the file it would help you more.

[CNCZACK]

18 minutes ago, AMCNitro said:

Trying to upload and it wont let me. 

First, use only the 3/8 tool and do a dynamic with the big circle set as AIR, you can do it in one shot with one tool, forget the 1/2 endmill. -

To do the radius use a flat endmill with the Flow Line, it will leave a sharp corner.  It works, I've done it dozens of time.

One more thing, use filters.  Don't forget the filters.  Did I mention filters?

Don't be afraid to do surfacing with flat endmills.

IF I could upload the file it would help you more.

this is almost exactly what ive got going on right now. filter are always so weird for me. I set them in the .003-.005 range and at 50% and saves some on this style program but ill try the 3/8 on the rad. i cant seem to get it to flow in the rest of the part and blend now 

[AMCNitro]

You had one dynamic coming in from the inside and one from the outside.  The way I did it is one operation with the 3/8s tool and setting the inner diameter as air, using the 1/2 then the 3/8s is a waste of time IMO.  Also, I don't mess the filter tolerance.  See the thumbnail to see how I do it.

I use the same filter settings for dynamic operation and for the flowline

[CNCZACK]

28 minutes ago, AMCNitro said:

You had one dynamic coming in from the inside and one from the outside.  The way I did it is one operation with the 3/8s tool and setting the inner diameter as air, using the 1/2 then the 3/8s is a waste of time IMO.  Also, I don't mess the filter tolerance.  See the thumbnail to see how I do it.

I use the same filter settings for dynamic operation and for the flowline

sorry wasnt referring to what i posted before, i meant what im working on now. ill attach what ive got so far. Ive broken it up to prevent using import nci lol. Also i didnt know flowline had an arc filter page! where's that at?!

mill internet.mcam

[AMCNitro]

All surfacing TPs have filters, plus all the dynamic TPs

That's actually pretty good, having to deal with small memories, that's probably the best you can do.

What material is the part made of?

[CNCZACK]

2 minutes ago, AMCNitro said:

Well that helps a ton, thanks!