Surface Plunge Rough

[unhappyuser]

Has anyone had any success with this tool path? First time I have using it and it seems that it does not give me many options of how to control where I want to start and stop. I am trying to plunge a slot 8 inches deep by 2.25 inches wide with a .75 corner radius at the bottom. Many tool techs suggest plunging down and feeding away from the wall, and not going down to the same depth each time you step over. Only options I see is helix and peck. I am using x6 (mu something version). The material is A514 tool steel with flame cuts on the out side profile.

[Dan@home]

If you make a (dummy) pocket tool path with the same area, step over, pattern, lead in/out and tool dia. as you need for the plunge tool path. No depth is needed, just flat on the top of your part.

 

In the parameters of the plunge tool path, it has a option of using the nci from another tool path. Select the dummy tool path you just created above the part. It will have the same path as the dummy, only it will plunge. You can change the plunge by changing the dummy. Asume tool path.

 

About the feeding away from part. I don't think it will do that, I could be wrong. The surface Rough Flow line will do that.

[unhappyuser]

Thank you for your advise. I've tried that too. I've tried many things but to no success. It still wants to start where it wants. Some times mastercam wont give you the toolpath you want because the part geometry is just odd. I am just so frustrated with the soft ware now. Also the owner of my company is too. We've been using mastercam since version 5, and sometimes just for the software to do the simplest things, it wont do it. It's like screw you I dont want to do it. I want to be able to use these supposively awesome tools and tool paths, but I cant. It's been almost a week since I've contacted tech support. Still waiting for an answer and some help. But the time they figured it out I've probably figured out a different way to finish the part and shipped it already.

[gcode]

It still wants to start where it wants

 

draw a point where you want it to start

when you chain the dummy pocket toolpath, chain the point first

[Dan@home]

"It's been almost a week since I've contacted tech support." I find most of the times it is faster to get answers here. Answers here can come at the blink of an eye, depending on the day you ask.

 

As gcode said. Also you can put the point out side the pocket and the path will start there. Sometimes you may need to change your lead in/out to start at point or turn it off..

[Colin Gilchrist]

Please send in an enhancement request to QC for the back off move in Plunge Roughing. That has always been a feature that is lacking. The Advanced Multiaxis Toolpath has a Plunge Rough option that includes a "slide move" at the bottom of the plunge, but I couldn't get the slide move to go perpendicular to the cut direction, so it still doesn't keep the inserts off the walls.

 

Your best bet is to use a pocket Toolpath as others have mentioned as the "source" for the plunge motion, and turn off "Rapid retract". Then set your retract feed to about twice your cutting feedrate. Try not to go above 80-100 ipm on the retract to avoid dulling the inserts.

 

What diameter of cutter are you using? Since your slot is so wide, I'd be tempted to use a Feed Mill cutter instead of plunging. You could get a 1.5-2.0 diameter Feed Mill and you would only need 2 passes per depth cut. Sure, you are only cutting a very shallow depth of cut, but at high enough feeds to make up for it.

 

Hope that helps,

 

Colin

[unhappyuser]

Thank you for your input. I will try with the pocketing dummy program when I get into work in the morning. High feed is an option, but the pocket depth is so deep that it doesnt help. Max rpm on my machine is 2500 rm. 50 taper boring mill. rough pluuging the pocket out 8 inchess deep with a .75 corner radius on the bottom x's 2.25 wide. Most of my material is out of there already from drilling with an inch and a half inserted drill. and the walls are semi finish about 4 inches deep. Ok heres a rough dimenson of my slot. 8 inches deep x's 2.25 wide x's .75 corner radius so that gives me a bout a .75 flat area on the bottom and its about 18 inches long. Due to these dimension I am down to an 1.25 Sandvik plunge mill to rough out the rest of the material.Now finishing will be another night mare, but I am sure I will just crawl through there with a long extension inserted cutter. Start with a short one and work my way up until I get to full depth.

[unhappyuser]

I used the pucketing dummy program and it starts where I wanted. Worked out great. Thank you. BTW tech support never got back to me yet...................

[gcode]

happy to help

[dforsythe]

Has anyone had any success with this tool path? First time I have using it and it seems that it does not give me many options of how to control where I want to start and stop. I am trying to plunge a slot 8 inches deep by 2.25 inches wide with a .75 corner radius at the bottom. Many tool techs suggest plunging down and feeding away from the wall, and not going down to the same depth each time you step over. Only options I see is helix and peck. I am using x6 (mu something version). The material is A514 tool steel with flame cuts on the out side profile.

 

It works great when you have the corect aplication. the key is having the tool vector away from wall during retracts to prevent the insert from getting damaged. this would be a great option for MC to look into.

[Rob Dusenbury CAD/CAM CONSULTING]

Use the direction button on the surface parameters page. You can set the retract amount and angle there. Also max step down and cut depths should help you with depth cuts.

[Rstewart]

Use the direction button on the surface parameters page. You can set the retract amount and angle there. Also max step down and cut depths should help you with depth cuts.

 

If there was a "cut from one direction only" button this would work. It will rapid into material one way and work fine when the tool goes back the other direction. just tried it.

[Rob Dusenbury CAD/CAM CONSULTING]

Try an xy angle of 270 or 90 depending on the direction of your first cut. I agree it should have more control, but if you get the retract angle to retract into your last row you should be fine. It also uses a feed move not a rapid move. The point is, it has been here all along, just nobody ever tries it. Hope this helps.

[rogkick]

The direction tab options work perfectly well, after you play around with the angles. I used it, and was moderately satisfied with the result.

[brandon b]

I used this path a year ago. The direction control worked fine for me. Like what you all said just need to play around with it a little.

[brandon b]

retracts back then up

[Rstewart]

Ok I stand corrected! Thanks guys, I'll give this a go next time i have an app for this path