Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Helix bore start


Brian Pallas
 Share

Recommended Posts

I've noticed before if I use the helix bore with "start angle" and "entry/exit arc sweep" set to 0. (see screenshot 01), that the toolpath isn't starting at an angle of 0. (see screenshot 2).  I have to make the start angle different by how much off the tool wants to start, which here is 330. (see screenshot 3),  to get it to start at an angle of 0 (screenshot 4). And it doesn't seem to be a constant number that it is off.

 

Changing the pitch on the "rough/finish" tab changes the startpoint of the toolpath also.

 

Never really dug into before why it does that, or how to control the start of the toolpath without playing with the start angle every time.  Is there a way to get that to behave appropriately? (the value in the start angle box is the actual value that is used) 

SCREEN01.png

SCREEN02.png

SCREEN03.png

SCREEN04.png

Link to comment
Share on other sites

I always use entity, but if the arc was drawn using a rotate/copy the start point rotates along with the entity. This was true with curves generated on a customer model too

 

You can draw arcs on a different level (not rotating them) and they will all have the same start point

Link to comment
Share on other sites
15 hours ago, jeff said:

+1000000001

+1000000002

 

I had this happen just a few weeks ago at a customers on a new Okuma MB-4000H. I was in a hurry and selected the solid curve and the lead-in/lead-out was at an odd angle. I didn't put much thought into it and turns out the edge was broken into four quadrants, no big deal but they were of deferent radius. the bore was out of round by .004" and I was standing there trying to explain there is no way a new machine could be off that bad. After hours of trying to figure it out, looking over the code and spotted the issue, went back to Mastercam and the model was bad. The machine did what I told it to do. I re-created a circle with a point and never again will I interpolate a bore from the solid without checking it first.

  • Like 1
Link to comment
Share on other sites
1 minute ago, Tim Johnson said:

I always use entity but I set my start angle at 90, entry/exit arc sweep at 90, start at center checked, and perpendicular entry unchecked. It always starts at the center point of the hole. It really doesn't matter what the start angle is though.

Yup except I use perpendicular entry and entr/exit @ 15.

Link to comment
Share on other sites

Weird, I started a new file today to play with this some more, and the start angle thing is working...basically.  I did that the other day and was having the oddness that I originally posted about.  Today putting in a start angle of 0, 90 , 180 , 270 had it starting at the quadrants, except it's rotated by 180 (a start angle of 0 should be at 3 o'clock but it's starting at 9.)   Which is odd, but that's fine.

It doesn't matter for the machining being done, but looking at the code is a lot easier if the arcs are starting at the quadrants.  When I am scanning the code for a program I like to be able to easily figure out what diameter arc is programmed.  I started using center points only quite a few years ago, was much more reliable for me, but you do need to enter in the diameter to be machined, which is a source of error.  So I like to double check the code to the print.  So that's at least why I do that.

 

 

 

 

not at quadrant.png

at quadrant.png

Link to comment
Share on other sites
On 5/31/2017 at 3:04 PM, #Rekd™ said:

Not sure if it changes anything but does driving the tool path from geometry vs a point make any difference?

I almost always use a point.

 

 

The only difference that I've found is that when using an entity, you're locked in to whatever size that entity is. When using a point, you can enter any size for a hole diameter.

Link to comment
Share on other sites
Just now, Ocean Lacky™ said:

The only difference that I've found is that when using an entity, you're locked in to whatever size that entity is. When using a point, you can enter any size for a hole diameter.

Yes but using entities I can machine MANY different sizes in one path

Link to comment
Share on other sites
1 hour ago, JParis said:

Yes but using entities I can machine MANY different sizes in one path

But Mastercam will allow you to have one size defined and not greyed out the diameter box if you mix and match by accident or thinking you are grabbing a feature that is the same size as what you are trying to cut with the points and it is not. So the programmer is thinking they have programmed using only points and they are all that size or they have programmed using entities with the understanding the diameter box is greyed out, but when you make a mistake and the process is not predictable do you take the time to go with a proved step by step process that does allows the programmer to define the process and size through more operations or do you roll the dice and hope you didn't pick the wrong size entity and get holes that may be cut different than you thought because the system is not telling you what size you are cutting on each size entity?

I just made this mistake getting in a hurry trying to listen and use entitles. I quit doing it years ago because it is not a fail safe process. I use points and yes it is more work, but when it has to be correct and human error is not be accounted for even through the Verification system then I must go with a process that checks for human error by using points. With entitles you can pick smaller entitles and on something with 20,000 holes how do you find the one that was smaller if some of them have multiple size entities for one feature? Again lucky I went to the small size, but had I gone over size on my process I would have caught it for the holes in the Verification, but not for the treadmills since all thread milling in a Verification program is a gouge when the model is to the tap drill size not the finished threadmill size. The only way to get around it is to make a finished thread size hole on all ID tapped features that you then use in your verification program which is more work than just using points and know what you know.

Link to comment
Share on other sites
10 minutes ago, C^Millman said:

 or do you roll the dice and hope you didn't pick the wrong size entity

I've been burned too many times by rolling the dice. Now I always take the extra time to pick points and enter in the exact size I want the hole to be machined to.

I'd rather have 20 different circle mill toolpaths and have them be correct than guess with 1 toolpath for different hole sizes.

 

Picking points also allows for quick and easy engineering changes or Revision changes down the road..which happens quite often from some of my customers.

  • Like 1
Link to comment
Share on other sites
6 minutes ago, Leon82 said:

Many ways to skin the cat, I've also been in a hurry and pick the edge of the hole instead of the center using points

I got badly burned by this in early X days... which is why I started using enties

  • Like 1
Link to comment
Share on other sites
48 minutes ago, Leon82 said:

Many ways to skin the cat, I've also been in a hurry and pick the edge of the hole instead of the center using points

Agree, but if you use the hole axis and only make points on a separate level. You can then use the lock to points in auto cursor and now will pick only those center points and done. Much easier to see a hole on a quadrant picked wrong than an entity that may only be .005 smaller or larger than the size you were expecting to pick. 

 

Link to comment
Share on other sites
Just now, BrianP. said:

Curious as to how often you guys use this path. I hardly if ever use this path. Circle mill all the time but very rarely this one. Where would you use this over circle mill path?

All the time to machine a hole. Ramping into something is much better than plunging. I will use circle mill sometimes to finish a hole, but since you finish a hole with helix no issues there.

Link to comment
Share on other sites
27 minutes ago, C^Millman said:

All the time to machine a hole. Ramping into something is much better than plunging. I will use circle mill sometimes to finish a hole, but since you finish a hole with helix no issues there.

But you can ramp with circle mill. One of the reasons I have always found this tool path to be kind of redundant .

Link to comment
Share on other sites
8 minutes ago, BrianP. said:

But you can ramp with circle mill. One of the reasons I have always found this tool path to be kind of redundant .

You can spiral out, helix down and circle mill all in 1 path.....Not another path like it in the software :)

Link to comment
Share on other sites
Just now, JParis said:

Circle......Helix doesn't have a spiral option for roughing

Ok. We are on the same page then. I use circle mill a ton. I do prefer to drill and drop straight in instead of spiral but use it either way. The roughing step over, semi finish and finish options make it a very versatile path. 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...