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:

Advice for Toolpath, Please


Bill H
 Share

Recommended Posts

2 hours ago, JB7280 said:

I applied this to a part I'm working on right now, and I really like it.  Although I don't love the entry/exits, but i imagine I can get those how I like them with some tweaking. 

 

I always forget about the possibility of using 3D toolpaths on 2D surfaces.  What other 3D toolpaths have this type of functionality?

All of them.

  • Like 1
Link to comment
Share on other sites
On 1/17/2021 at 5:46 AM, Bill H said:

DUM1: I like this!  The few snail trails are fairly symmetrical and don't bother me.  Are there any secrets to getting the toolpath to come out like this?

not  really much more then I already said in the previous post , messing with the step over changes the results, as far as the un uniform traces go .IMG_4291(1).thumb.jpg.035e1c83005358f4c4893d93099bd8d4.jpg

  • Like 4
Link to comment
Share on other sites

 

On 1/21/2021 at 9:53 AM, DUM1 said:

not  really much more then I already said in the previous post , messing with the step over changes the results, as far as the un uniform traces go .IMG_4291(1).thumb.jpg.035e1c83005358f4c4893d93099bd8d4.jpg

Hmm I have never tried that cut pattern for floor finishing but it looks really great for that application. Nice work!

  • Thanks 1
Link to comment
Share on other sites
9 hours ago, Bob W. said:

I like to finish floors with 2D HST and use a .002" micro lift and leaving .001-.002 on the walls.  I would then finish the boss walls using contour or waterline leaving .0005" on the floor so no witness marks.

Good strategy Bob, but if you are only leaving 0.001-0.002 stock on the walls, this will limit your filtering tolerance values.

In general, you want to be sure that your Cut Tolerance on the Filter page is around 10-20% of your Stock to Leave value. At 20%, and leaving the 'high value' of 0.002, your Cut Tolerance should be down around 0.0002-0.0004.

There is nothing inherently wrong with this approach, but there is performance to be gained from your computer hardware, by using a bit more 'Stock to Leave' on the walls.

Technically speaking, with a fast enough computer, this is a moot point. But I see many Mastercam Programmers who don't know much about adjusting the Filter, and they just end up using the Filter Default Values.

If you were to leave 0.008 Stock on the walls (0.2mm), you could safely put the Total Tolerance around 0.004, the Cut Tolerance at 0.001, and the Line/Arc Filter enabled at 0.003. (25% Cut Tol, 75% Filter Tol).

Within the Line/Arc Filter, there are options to control "how the tolerance value is 'split' between Linearization and Arc Creation".
 

 

 

 

  • Thanks 1
Link to comment
Share on other sites

When you open up the tolerance like that (0.004 total, 0.001 Cut, 0.003 Filter), there are 3 options on the Radio buttons below, which allow you control over how the filter is applied.

I believe that the "linear filter" is applied first, and then the Arc Filter is applied. For this reason, if you want to limit the amount of lines, and focus more on generating Arc output, you can use the 'Tighten Arc Filtering' Radio Button to do this. You then have a slider to control "how much of the tolerance is linear, and how much is Arc Filter"? In my example, where we are using 0.003 for the Filter Tolerance, I'd typically use the 'Tighten Arc Filter', and set it to 75% or 100%, using that slider. At 100%, you should mainly be creating Arcs for all the curved offsets geometry, for moves the 'filter' can actually do an 'arc fitting' to.

  • Thanks 1
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...