Straight plunge in 2D HST

[E300]

Good day all.. I was wondering how to plunge straight down in 2D HST (Eg: Core Mill)? I have been told to set helix & ramp to "0" still want to helix.. Put ramp to 90 and still want to helix????? Cheers

[Buddy J]

I hope you get an answer to this

I avoid using it for this very reason when it creates a ton of code doing moves I don't even want!

[Tyler Robertson]

Still helixes even if you set it to ramp, and 0?? Now that' strange. What version of mastercam?

 

X6 MU2 I set everything to 0 and it plunges down.

 

Try using an Approach/Retract point under Linking Parameters to se if it changes anything.

[kostiuk]

I don't know if it's the correct way to do it or not but I create a .002 line at the point I want it to plunge into. Then pick it as the entry chain. Then in entry motion choose "custom, use entry chain" for the entry method. Tell it a plunge angle of 90 degrees. Seems kinda clunky but it works. I hope someone chimes in with a better way.

Kevin K.

[Colin Gilchrist]

You can force 2D Core to output plunge moves by setting the Plunge Angle to 89.9 degrees (90 causes an error). Also, under the Linking Parameters, make sure you set the vertical entry/exit arcs to "0.0".

 

That said, the Dynamic Core path will produce better cutting conditions than the 2D Core Mill. 2D Core is the "legacy" 2D HST path, and Dynamic Core has been updated to use an improved algorithm for calculating the toolpath motion. Dynamic Core also readily accepts a plunge value of 90 degrees, with a Helix Radius of "0.0". (straight plunge).

[kostiuk]

But how do you get it to plunge where you want it to and not where it wants to?

[K2csq7]

But how do you get it to plunge where you want it to and not where it wants to?

Not sure about the dynamic paths, but for the some paths you can put a point where you want it to plunge, then chain that point in the toolpath before your actual chain.... If this doesn't work, I backplot the path taking note of the entry point mcam starts at, then make my entry hole at that location.

[Colin Gilchrist]

"Core" milling is designed to cut a part from the "outside -> in", leaving features standing up like bosses. It is designed to plunge outside the material.

 

There is an option in Dynamic Core to choose "approach distance" and a drop down menu that lets you choose an approximate start point (the four corners, or four midpoints of a square around the part shape). This is not an exact location. There is no way to specify an exact location with the "Core" style paths. This is how they are designed.

 

If you need to plunge at a defined point, then try using the Dynamic Area toolpath. Expand your chain so that the entry point is contained inside the chain, and there is enough room to get the tool into that spot (if you are using a .500 endmill, you need to keep that entry point away from the chain boundary by the radius of your tool + a small amount of "clearance")

 

That allows you to add a "chained point" in your geometry selection, and you can enable the "Center helix on point" checkbox, set your Helix radius to 0.0, and your plunge angle to 90. That will give you a vertical plunge entry, and then start cutting the shape.

[left coast lefty]

"Core" milling is designed to cut a part from the "outside -> in", leaving features standing up like bosses. It is designed to plunge outside the material.

 

There is an option in Dynamic Core to choose "approach distance" and a drop down menu that lets you choose an approximate start point (the four corners, or four midpoints of a square around the part shape). This is not an exact location. There is no way to specify an exact location with the "Core" style paths. This is how they are designed.

 

If you need to plunge at a defined point, then try using the Dynamic Area toolpath. Expand your chain so that the entry point is contained inside the chain, and there is enough room to get the tool into that spot (if you are using a .500 endmill, you need to keep that entry point away from the chain boundary by the radius of your tool + a small amount of "clearance")

 

That allows you to add a "chained point" in your geometry selection, and you can enable the "Center helix on point" checkbox, set your Helix radius to 0.0, and your plunge angle to 90. That will give you a vertical plunge entry, and then start cutting the shape.

 

+100000

 

This is exactly the way I do it.

[kostiuk]

So I'm having trouble with this. Using Dynamic Area Mill I select the chain then pick multiple machining regions then pick entry chain and pick the point. After I do that it does not show any entry chains on the chain options page but I continued with the program anyway. For entry motion I choose helix only, 0 radius, and plunge angle of 90 degrees. It starts wherever it wants. What am i doing wrong?

 

Thanks, Kevin K.

[Colin Gilchrist]

Don't pick the multiple machining regions. This tells Mastercam you want to cut in multiple areas.

 

Start the toolpath, and select the outside boundary chain. Then change your chaining mode to "Point", and select your entry point (note: that could be an actual point entity, or an arc center, endpoint, ect). When you press the accept button on the chaining dialog box, you should see the Chain Options, with 'Single region' selected. It will show the number '2' next to the selection arrow button, indicating that you have two chains selected.

 

Now set your entry options, including '0.0' helix radius, and '90.0' for the plunge angle.

 

Note that there is also a 'Chaining selection arrow' button on the 'Entry' page, which allows you to go select an entry point "after the fact". So if you only selected a single chain initially, but want to add the entry point, you can do that directly on the entry page...

[Colin Gilchrist]

One thing I recommend doing is creating an arc entity where you want the entry point, that is bigger than your cutter diameter. This ensures that if you use the arc center as the entry point, your tool can actually fit inside your boundary chain.

 

For example, I'd use a .85 diameter arc if I was planning on cutting with a .75 diameter endmill. As long as the entire arc fits inside your boundary chain, the entry motion should not fail. (Just a tip/trick I use)

[kostiuk]

Sweet. That works perfectly. Thanks, Colin

 

Kevin K.

[Colin Gilchrist]

Sweet. That works perfectly. Thanks, Colin

 

Kevin K.

 

You are welcome Kevin, I'm glad it is working for you. One thing i noticed the straight plunge move is it creates a lot of very small linear moves at the start of the spiral motion. I'd recommend turning on the toolpath filter to help simplify the code.

 

Out of curiosity, are there specific reasons anyone is trying to use a start point? The ramp or helix entry methods tend to work very well, and save you a tool change. The entry motion had separate speeds and feeds, and also allows you to program a dwell before starting the normal cutting motion.

 

I did see an enhancement request for harder materials like titanium and HRSA that would have the tool back off the wall before the dwell occurs, to prevent the tool from rubbing (a great idea!), but I'm curious what others think. I've had great success using the 2D HST paths without an entry hole, by using the existing entry options.

[Glenn Bouman]

Out of curiosity, are there specific reasons anyone is trying to use a start point?

 

When the part has a existing opening (casting) or a pre-drilled hole.

[mayday]

The ramp or helix entry methods tend to work very well, and save you a tool change.

 

Colin, that's great for plastic and aluminum

 

tool life comes to an end in high nickel alloys. starting off the part is a must or a drilled entry hole.

[K2csq7]

All we do is Superalloys, Insert drills are the way to go, drop to depth and the first time the tool contacts the material it is in the dynamic motion. If you ramp or helix in the bottom of the tool gets worn out quicker than the rest of the flute. May not be much, but any imperfection in the cutting surface of the tool will kill it within seconds...

 

Ramping does work well with the right tools, but tools wear so quickly in superalloys as it is, you cant afford uneven wear on your tools.

[kostiuk]

Same for us as the other folks said. A lot of times we may need to have holes in the part any way so we might as well plunge into them. We really are just starting to use these paths in our mold base work. We had trouble getting chips out of the hole as it did its helix and the bottom of the cutter really took a beating. We may play with our speeds and feeds some to try and fix that.

 

Thanks again, Kevin K.

[Colin Gilchrist]

Great replies, and I'll put in an enhancement request to make it easier to plunge into a pre-existing hole.

[left coast lefty]

Great replies, and I'll put in an enhancement request to make it easier to plunge into a pre-existing hole.

 

Excellent!

 

Now that we're on the subject, how about multi-threading for 2D HST? I started a thread awhile back, got lots of support but no action.

http://www.emasterca...ulti +threading

[Newbeeee™]

Excellent!

 

Now that we're on the subject, how about multi-threading for 2D HST? I started a thread awhile back, got lots of support but no action.

http://www.emasterca...ulti +threading

Haha - in for a penny and in for a pound!

[left coast lefty]

Haha - in for a penny and in for a pound!

 

Just Yankee ingenuity- oh wait............!