Problem with Dynamic Core Milling

[Thad]

Thad, check out Chris' signature: ..(Google Chrome will freeze the first column, IE and firefox won't)

 

Just use Google Chrome to view the spreadsheet, and the first column freezes...

 

Thanks Colin. I read that yesterday and took it as Chrome had a bug that caused it to freeze (lock up). I didn't care because I use FF. DOH!

[cobra95kev]

Colin,

Thanks for posting those toolpaths. I didn't know that was possible. One question, what about the back feedrates when it is out of the cut? Is there any way to speed them up? I tried a few things and could get nothing to work?

 

Thanks,

Kevin C.

[jeff]

 

what about the back feedrates when it is out of the cut? Is there any way to speed them up?

 

There is a box for setting the back feedrate. 

[cobra95kev]

I was talking about in the toolpaths Colin posted on his files he uploaded. The mesh toolpaths.

 

Thanks,

Kevin

[Colin Gilchrist]

Colin,

Thanks for posting those toolpaths. I didn't know that was possible. One question, what about the back feedrates when it is out of the cut? Is there any way to speed them up? I tried a few things and could get nothing to work?

 

Thanks,

Kevin C.

 

Hi Kevin,

 

There is an option available to control this, but it appears to be broken. Check under the "Utility" page. There are options to output feedrate values for the different linking move types, but the feed value does not appear to change when I backplot the toolpath.

 

 

[Luke.Hicks430]

Has the OD Corner stepover problem been addressed with newer versions of mastercam?

The main problem I run into is using high-flute-count endmills. The Imco 9fl endmill has a maximum of .05 radial DOC. This means I would have to set my dynamic toolpath to use a stepover of about .015 to not violate the .05 maximum DOC. I'm not able to use my tool to it's fullest abilities. It would be nice to have a solution to this.

I'm running X6. 

[crazy^millman]

20 minutes ago, Luke.Hicks430 said:

Has the OD Corner stepover problem been addressed with newer versions of mastercam?

The main problem I run into is using high-flute-count endmills. The Imco 9fl endmill has a maximum of .05 radial DOC. This means I would have to set my dynamic toolpath to use a stepover of about .015 to not violate the .05 maximum DOC. I'm not able to use my tool to it's fullest abilities. It would be nice to have a solution to this.

I'm running X6. 

Need to look into 2018 Mastercam. That version was just getting it's feet wet with HST toolpaths. The software has advanced and progressed with regards to area that they are in my opinion night and day software. Yes the Ribbon is a shock and take some time to adjust to. I din't say it was better I said adjust to.

[Luke.Hicks430]

2 hours ago, C^Millman said:

Need to look into 2018 Mastercam. 

I would love to, but I don't control the budget.

[Colin Gilchrist]

"Has the OD Corner stepover problem been addressed with newer versions of mastercam?" - YES. The issue has been addressed in newer versions of Mastercam's 2D and 3D paths. So updating to the latest version is worth the money.

 

With X6, you need to do some "Work" to get a path that gives you what you want.

With a "Rectangular piece of stock, I would recommend creating some Contour paths, just to rough the corners away. Do this as a separate operation, prior to cutting the 2D or 3D Dynamic paths.

To get good results, you'll want to either use a "big corner radius" or a 45 Degree Chamfer.

You can then use "Trim Toolpath", to trim away the excess "contour" motion. This gives you a "fairly efficient" method of knocking off the corners from the block of material.

When you use the 2D Dynamic to do your actual Roughing, you can then use the boundary that has the corners removed. I would still back off from whatever the "max" radial immersion value is. If you can only have a max radial engagement of .05, then I would program the path at .04 stepover, just to give it some wiggle room. The path will still be nice and efficient...

[Luke.Hicks430]

Colin,

Thank you for the advice, I think that is a god approach. Any tips on how to trim the corners of the stock before the Dynamic in a way that doesn't kill my tool, or just go for it as a contour?

I'm pushing for MC 2018 but it's a large chunk of change for a 25-person shop. I know it's worth it, but I think the hold up is cash flow. For now I make due with X6.

[Colin Gilchrist]

Example, take a 6" x 4" block, for example.

Put a 1" chamfer on all 4 corners. Use Chamfer, with "No Trim" active.  (put those lines on a Tool Path level)

Copy those lines to another level. Create two lines, parallel to the edges of the rectangle, and make the parallel distance 70% of your diameter. So I'll create two lines, .500 parallel. Then trim these lines to the 45 degree Chamfer line.  You are drawing a Triangle, that surrounds the corner, but has 2 sides offset a distance away.

Now, create a Contour Toolpath, and chain just the "45 degree" lines that are on the corner of the Triangle you just created.

In the Contour Path, make sure you use "extend start and end" of Contour, in lead in/out. Disable any other lead in/out motion, besides the "extension".

Enable "Multi-passes". Set "0" rough passes, and 14 finishes passes, at .05 stepover. Set your Speeds and Feeds to your "Dynamic" values. (fast)

Now, this creates a Contour Tool Path, that has the first pass cut "mostly air", and just nibbles the "tip" off the corner of the actual part.

This is where the "Trim" toolpath option comes in. Right-Click in your Ops Manager, and choose Mill Toolpaths > Trim.

Select the Triangle as the "trimming boundary". Select the corner of the "rectangle" (inside the triangle) as the "bias point". Set the option to "Keep Tool Up". (Set your Retract and Feed Planes as necessary for proper clearance. Pick the Contour Tool Path as the one you want to trim. (can only trim 1 at a time...)

What this gives you is a nice way to write a quick Contour path to cut off the corners of the block.

With the corners cut off, I take that new "outside boundary", and offset it by .1-.25. Then I create some "large fillets" between the sharp corners. Depending on the starting shape, sometimes it is worth it to just draw an Ellipse. Even if the tool cuts some air going around the outside, it is better than blowing up an expensive carbide tool.

 

 

 

 

[David Colin]

I never used X6 and its dynamic toolpath but in 2018 I guess you will still notice over 'radial' engagement in corners.

However, it's already been discussed here but Mastercam dynamic toolpaths GUI is not really clear about its stepover engagement textbox. Value typed in this field will only be used to calculate tool 'angle' engagement this way:

Tool engagement angle = COS^-1( 1 - stepover / tool _radius).

Dynamic toolpaths are all about tool engagement angle to maintain as constant as possible anywhere in toolpaths. This, for any CAM softwares.

IMHO, Mastercam, should add a textbox to show or even type-in tool engagement angle relative to stepover to make things clearer. Knowing that, if you experiment, you will see that this tool engagement angle will be maintain in any point of toolpath,  even in raw block corners.

[Martin.Chang]

Sorry I have bad news

this problem is not fixed with newer verison of mastercam

I'm running mastercam 2017 and  2018